CamBam

FeedBack => CamBam plus feedback => Topic started by: 10bulls on July 30, 2010, 19:02:09 pm

Title: CamBam plus 0.9.8
Post by: 10bulls on July 30, 2010, 19:02:09 pm
If anyone has any bug reports, comments or suggestions regarding the new CamBam version 0.9.8, please post them here.

Thank you very much for your feedback!  :)

Details of the new release and a link to the download are in this thread:
http://www.cambam.co.uk/forum/index.php?topic=1196.0
Title: Re: CamBam plus 0.9.8
Post by: kvom on July 30, 2010, 23:20:36 pm
I just installed, and it looks good.  I'll try to remake a part that I did with 9.7.

One suggestion is to put the CB version # in the first line of the g-code output.  I modified the post processor I use to reflect this.
Title: Re: CamBam plus 0.9.8
Post by: spiked3 on July 31, 2010, 01:28:46 am
I do not do the fancy machining a lot of others do, actually I have taken a break from doing much of anything for the moment - but;  I did do a chassis for a mobile robot and everything worked perfectly. I really like the new style paradigm. It also looks like some intelligent tool speed and feed type functionality is just around the corner as well, that is great.
Oh, and I love the ability to define (multiple) stocks and easily manipulate origins - it made the robot chassis go a lot faster than before since the part was too big for the machine and I had to break it into several localized operations - bravo.

I mentioned to a few already - but I will be posting the source for my Alibre to CamBam bridge (ver 0.9.8 compatible) again very shortly - it is actually already done :)  But I will not be able to offer any support for it. That was my intentions before and I lost track of that and it started taking a significant amount of time.

Andy, much thanks - Mike.
Title: Re: CamBam plus 0.9.8
Post by: coolant slinger on July 31, 2010, 13:31:27 pm
Andy,

I downloaded version 0.9.8. I see you added lead out to profiling tool path. This is nice. I also see that there is a lathe option and an example cb file of the lathe option. I do lathe work on my mill so this is a great addition to the software. I liked Lazycam for that very reason that it was capible of lathe and mill 2.5d. But it is not as powerfull and user friendly as CAMBAM. And they have stopped development. I can't wait to play with the lathe option. Dude, you just exceeded my expectations.
Keep up the good work.
Title: Re: CamBam plus 0.9.8
Post by: kvom on July 31, 2010, 14:10:04 pm
I did some experimenting with the tool libraries and ran into some minor issues.

1) When I create a new tool library, I cannot rename it.  First is named Tools, then Tools1.

2) When I added a tool to the library and referenced it in a pocket MOP, I got the error message Stepover must be greater then zero.  However, I had set stepover to .5.  When I just set the endmill diameter in the MOP (overriding the tool library), the message went away.  FWIW, it would be helpful if the name of a MOP is displayed with such error messages.

While I can select multiple MOPs, the enable/disable options don't work on the selected grouping.

I appreciate the new ability to generate G98 for clearance/retract height management in drilling.
Title: Re: CamBam plus 0.9.8
Post by: Jeff_Birt on July 31, 2010, 16:29:05 pm
One minor thing I have noticed is that the MOP window is reset when you generate a tool path. This is frustrating when you trying to get a setting just right and have to keep going back down the MOP window finding and expanding the correct section of the tree to make a minor tweak.
Title: Re: CamBam plus 0.9.8
Post by: EAC on July 31, 2010, 16:35:22 pm
Andy, you may already have some of these from DW testing   ;)  Just wanted to get them all in one place.

Can not rename any new Cam Styles....  just template1 etc... as with tool library.

It would be nice if style variants were shown under the original, (with the + ) instead of in the list separately.  Have not found a way to re-order the styles in the list.  They won't drag. No problem, just messy.

Made a new Cam Style (templates), and created a new style in it.  Applied the style to a MOP, and when I generated toolpath, it couldn't find the style.

When you set a new start point using the property method the tabs don't reflect the change as they do when start point is changed using right click method.  Would be nice to change to both calling the property method.

It would be nice to add a property to tabs that set the minimum distance from a endpoint (i.e.: corner).  Tabs too close to a corner always have to be moved.

Going to be working on stuff today, so I'm sure there will be more.. ;D

Don @ EAC
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on July 31, 2010, 19:27:56 pm
In my opinion, the hardest thing to grasp is where some of the settings or values within a MOP are being obtained and why.
If you've set MOPs to derive settings in several ways, it can soon get tricky to follow.
I think some kind of feedback would be in order, even if it's just colour co-ordinated text for a value that indicates the source Style is from a Part or Machining object.
I'd find it handy if the chosen Auto, Default, Value and Inherited option could remain on view in the MOP as well, to serve as a clue.
It would also save a couple of clicks if the Inherited style info could be displayed on the initial right click - if you get what I mean.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: FatFreddie on July 31, 2010, 21:52:37 pm
Nice one Andy - looks like lots of great improvements. Particularly pleased to see the lathe stuff. Unfortunately I'm off on holiday so won't get chance to play with it for a couple of weeks :-(

One minor comment - the MachiningOrigin defaults to NaN - is this by design?

Cheers,
Mark
Title: Re: CamBam plus 0.9.8
Post by: EAC on August 01, 2010, 02:59:52 am
A minor weird one that may be left over from 97, not sure..

Create a MOP, adjust tabs to your liking, then set a new style to the MOP.  The tabs stay set at manual.  This is a problem when you change to a style that has NO TABS.  Shouldn't tabs reset to the new style?  A new style should reset the MOP to NEW beforehand. We need to know that things won't be leftover if we make changes. That can cause a lot of problems.

Don @ EAC
Title: Re: CamBam plus 0.9.8
Post by: EAC on August 01, 2010, 03:11:59 am
OK, 1 more for Andy. :P

CB files convert to v98 when loaded, is there a way to 'apply to MOP' to copy old templates into styles?  Some of us have accumulated a lot of templates, and I can see a lot of typo's if we have to do it all manually.

Don @ EAC
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 01, 2010, 11:01:58 am
A minor weird one that may be left over from 97, not sure..

Create a MOP, adjust tabs to your liking, then set a new style to the MOP.  The tabs stay set at manual.  This is a problem when you change to a style that has NO TABS.  Shouldn't tabs reset to the new style?  A new style should reset the MOP to NEW beforehand. We need to know that things won't be leftover if we make changes. That can cause a lot of problems.

Don @ EAC

Don.
I think you might be running into the problem I'm referring to in my post above.
If you right-click on the words in the HoldingTabs cell of your MOP, you'll get the options of Auto, Default, Value and Inherited style. Try experimenting with these and see if it now works as you want.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: EAC on August 01, 2010, 19:34:29 pm
A minor weird one that may be left over from 97, not sure..

Create a MOP, adjust tabs to your liking, then set a new style to the MOP.  The tabs stay set at manual.  This is a problem when you change to a style that has NO TABS.  Shouldn't tabs reset to the new style?  A new style should reset the MOP to NEW beforehand. We need to know that things won't be leftover if we make changes. That can cause a lot of problems.

Don @ EAC

Don.
I think you might be running into the problem I'm referring to in my post above.
If you right-click on the words in the HoldingTabs cell of your MOP, you'll get the options of Auto, Default, Value and Inherited style. Try experimenting with these and see if it now works as you want.

Martin.

Yeah that fixes it once, but that setting changes with the new MOP applied, so it will be a problem again..   Maybe the 'Great One with the Beer Hat' will chime in on the logic for this issue.  Totally resetting the MOP before applying a new style is the only way I see it not getting in the way big time.

Don 
Title: Re: CamBam plus 0.9.8
Post by: EAC on August 01, 2010, 19:41:29 pm
Found the issue with not finding the MOP under new cam style 'templates'.  To find it is other than 'standard', you have to set the proper style folder in the 'style library' under 'part1'...  Then it won't find others under different sub-styles.

There is SO MUCH new in this version, that I can see it taking a while to get it all together, but it will be worth the wait.  Gonna be VERY cool, Andy :)

Don @ EAC
Title: Re: CamBam plus 0.9.8
Post by: kvom on August 01, 2010, 20:28:56 pm
The default for Spindle Direction in the provided styles, IMO, should be CW.  The first g-code I generated with 0.9.8 had no M3 code.
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 01, 2010, 21:14:31 pm
I think everything is working as designed, but we could do with a few more clues about where the data for each option is being got from. Maybe a breadcrumb trail kind of tool tip?
That's what I was trying to get at in my original post.
It's a lot more powerful than previously but it's a bit more complicated too.
You can have a Style in the Machining folder, Parts and any, or all of the MOPs - all at the same time and in any combination, along with any other tweaks - whether it makes sense or not! This is what threw me at first and still does on occassion.
Oh, and a Style can have a Parent Style as well :)

Martin.
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on August 01, 2010, 21:58:07 pm
Thanks for the great feedback guys.  I will certainly be referring back to this thread.

The response to the new style system is kind of what I was expecting.  I agree, with just a few simple relationships it is surprising how complicated things can quickly become.  I think some tutorials and a video tutorial will help some what.  I also agree that some refinements to the user interface would help with the problem of identifying where values are inheriting from.
Right clicking on a machining operation's property name reveals a context menu with an 'Inherited style' option.
It is very rudimentary at the moment, but this should show the style that a property is inheriting a value from.
I like the breadcrumb tooltip idea, I think that would work well.

Some brief responses previous comments:

Renaming style libraries / tool libraries.  This is on the todo list and will be done before we get to stable release status.

Listing child styles beneath parent styles.  I have considered this and I agree that it would make a nice way of managing style heirarchies and also make it visibly obvious which styles derive from what.  I just need to type faster! :)

MachiningOrigin showing NaN.  This is intentional (if a little ugly).  This way I can mark a point as 'Undefined', so that it knows to look up a level for a machining origin.  In later versions, the plan is to extend the use of the 'Default/Auto/Value' type properties to objects other than MOPs, so then the MachiningOrigin could just be marked as 'Default'.


Title: Re: CamBam plus 0.9.8
Post by: 10bulls on August 01, 2010, 22:02:25 pm
The default for Spindle Direction in the provided styles, IMO, should be CW.  The first g-code I generated with 0.9.8 had no M3 code.

I agree with you...but I can't seem to replicate this one.
The default spindle direction should be CW and the default spindle speed should be 1000.
I am not sure why you aren't getting an M3 in your post.... If you have a .cb file, I can check this out.
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 01, 2010, 22:14:43 pm
First Impression: very good job and biggest thanks to andy.
Without any details it will need some days to understand the new template system.

While first playing I found 2 bugs with the Menue -> toolkit.
With the the timing pulley and the involute gear I become an error: "Method not found: Void CamBam.CAD.Entity.Apply Transformation()".
The Details in the attachment.
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on August 01, 2010, 22:34:59 pm
Oops!  :-[

Was actually a bug with the installer generation, not picking up the latest plugin.

I have attached the latest plugin DLL.  Unzip this into the CamBam 0.9.8\plugins folder and hopefully this should fix things.
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 01, 2010, 22:58:36 pm
 ;D Yes thank you, it works.
Title: Re: CamBam plus 0.9.8
Post by: kvom on August 01, 2010, 23:20:12 pm
The default for Spindle Direction in the provided styles, IMO, should be CW.  The first g-code I generated with 0.9.8 had no M3 code.

I agree with you...but I can't seem to replicate this one.
The default spindle direction should be CW and the default spindle speed should be 1000.
I am not sure why you aren't getting an M3 in your post.... If you have a .cb file, I can check this out.

Might have been my fault playing with styles.  I solved the problem by setting CW in the default, unnamed, style. 
Title: Re: CamBam plus 0.9.8
Post by: lazer on August 02, 2010, 13:51:24 pm
Hi all

I did a micro tutorial for you all.
See in http://www.cambam.co.uk/forum/index.php?topic=1206.0

Armando
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 04, 2010, 20:50:01 pm
I open a DXF in CB.
I activate all objects (strg+a), then I drag all objects (shift+ mouse-drag).

While I drag, the splines going with the mouse, after I release the mouse on new place, splines are jumping back.
It drags only the polylines. After I convert all splines to polylines I can drag them also, but it is not possible to drag splines.
In 0.97 it is not a problem, I can drag also splines.

When I choose a toolnumber in the mop, for the tools I define myself, it set no diameter and no tool profile.
I can find no way, to define new tools that work the same as the sample tools.
How works it with the tool database?

And every time I choose a new mop CB prompts: Style''not found


thanks
ralf
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on August 04, 2010, 21:59:19 pm
I have just fixed the spline problem, so that should be sorted for the next release. 

A check list for getting the tool lookup to work:

Unless you have specified a ToolLibrary in the Machining folder or Part object, CamBam will look for the tool index in the library named 'Default-(units)', where units is the drawing units so for you most likely 'Default-mm'.

When you select the tool number in the MOP, does the name in the drop down list match your new tool?
This is a good test to see whether it is picking up the correct tool library.

The tool diameter and tool profile need to be set as 'Default'.  This is done by right clicking the ToolDiameter and  ToolProfile the selecting Default in the popup menu.
The tool diameter and profile should be displayed in grey italics to indicate they are being inherited.

If this still does not work, feel free to upload a file and I will investigate.

Has the style with an empty name '' been deleted?  This should exist in the default style library 'Standard-mm' for example.  This is a very important style as all styles will derive from this.
I should change the name of this style to maybe '<default>' and display warnings if you try to delete it.  Does this help?
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 04, 2010, 22:45:02 pm
Thank you for your fast answer,

Yes, shure, I deletet this very importet style. I am testing around to understand the new styles system. So I thought it was one I created and deletet it.
A warning prompt will be very helpfull.

Now I have reinstalled CamBam and all works.

The sample tools are back and working.
Tomorrow I start again with creating own tools ;D

This all with the new databases, for me is a bit difficult to understand.

thank you

ralf
Title: Re: CamBam plus 0.9.8 pocketing and DepthFirst
Post by: pixelmaker on August 07, 2010, 17:42:36 pm
Now I start milling testfiles made with cambam 0.98.
First today, some pockets.

When pocketing with option DepthFirst, it mills first the innerst toolpath till deepest level, then the next outer toolpath also till deepest level. It don´t finish the total level bevor going deeper.
It don´t cut one pocket after an other it cuts a toolpath after an other.

When pocketing with option LevelFirst he finish the total level, same as in V 0.97.


ralf
Title: Re: CamBam plus 0.9.8 next, profile tres bizard
Post by: pixelmaker on August 07, 2010, 20:46:26 pm
next I make a vacuumplate.
At first with 0.97, no problems

Then 0.98, I try to use the same values then in 0.9.7: Numbers shown at the foto.

1) cutting the profile-mop "dichtnut", a"bubble" is at the side of the regular toolpath.
2) Here he change the cutting-direction, must test that this is correct, and compare with 0.97, will do tomorrow, if it rains also and no motocycling is possible.

3 + 4)I made different mops for  the horizontal and the vertical slots. In each it cuts 1 slot incorrect. The slot 3 vertical and I think 4 horizontal it cuts at first the deepest level, then it goes to clearence plane, then it goes very slowly down on the first level an cuts some air.
All the other Slots it cuts correct.

ralf
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on August 07, 2010, 22:51:49 pm
Thanks Ralf, I will look into this.

I can't seem to make the 'bubble' appear on 'dichtnut'.  What controller software do you use?  This might be an arc precision problem... some controllers do not like very small arcs.  There is a setting in the post processor definition to set the minimum arc size (a straight move is used instead).  I can go into more detail if that may be the problem.

The 'Standard' optimisation mode *should* behave like 0.9.7 but there is definitely something going wrong there...I will investigate.
Title: Re: CamBam plus 0.9.8
Post by: kvom on August 07, 2010, 23:25:16 pm
First a question:  what is the difference between the PlungeFeedRate and the CutFeedRate for drill  MOPs?

Second, the field labels for LeadOutMove on Profile MOPs show Leadin for Type and FeedRate.
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 08, 2010, 00:35:35 am
hello Andy,
I use now WinPCNC economy but will change to USBCNC asap.

I use the post processor "default" in 0.97 and 0.98. The MinimumArcLength is 1e-4 in both pp.
There is only one difference between the two pp, that is a variable $k.



thank you

Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 08, 2010, 12:53:53 pm
Hello Andy,
so, if I understand the "times ten to the power of"-thing, it means that the MinimumArcLength 1e-4 is 1/10000 of a drawing unit and 1e-3 means than MinimumArcLength is 1/1000 of drawing unit.

For my mill with smallest step from 0,00625 mm and a repeat accuracy from 0,015 mm, I think there is no difference.

I changed now to MinimumArcLength 1e-3 and the "warts" have gone.

remains the thing with cutting the lowest level bevor the first in one of three slots,  for this I can´t find a solution.
It looks like a bug in DepthFirst

Thank you

ralf
Title: Re: CamBam plus 0.9.8
Post by: kvom on August 09, 2010, 12:35:33 pm
When I open a DXF in 9.8, the created layer is named "0" and the lines as shown in black, not the normal drawing color (green).  I can create a new layer and copy all the elements, and the color is restored.
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on August 09, 2010, 23:55:50 pm
When I open a DXF in 9.8, the created layer is named "0" and the lines as shown in black, not the normal drawing color (green).  I can create a new layer and copy all the elements, and the color is restored.

I can't seem to replicate this one.  Is it that the dxf file has the layer colour set as black?
It would be a good idea if CamBam detected files where the drawing colour was the same as the background
colour and adjusted it so it is visible.

If the DXF file should have a colour set, then if you can upload a DXF file I will investigate.
Title: Re: CamBam plus 0.9.8
Post by: kvom on August 10, 2010, 00:22:43 am
The file was generated from DeskEngrave, a program I learned about  on this forum.  It generates text along a curve, something CB cannot do at this point.  I am attaching the file.
Title: Re: CamBam plus 0.9.8
Post by: GeorgeRace on August 10, 2010, 01:09:58 am
Hi Andy:
Help, in production and am having a problem with a file that has worked just great for the past 2 years.
Attached is the .cb file.

First a minor annoyance that just cropped up this afternoon.

Load in the George Race Plate.cb file.  Then select one of the letters in the top line of text.  Press the delete key.  Box opens that says: Delete selected entities.  Now click on OK.  Next an error box opens that says:  Unknown Field/Property: MOPProfile._Tabs     When you acknowledge the error, the box closes and the highlighted text is erased.  Something is strange, but it does delete the object selected just fine.

Now for the real problem that has stopped me in my tracks this afternoon.

Load the George Race Plate.cb file in 9.8d.  Now expand Layer 1.  Click on polyline1.  You will see the portions of the emblem highlighted on the left side that belongs to polyline1.  Now Click on Produce G Code.  Load the produced .tap file into Mach3.  Zoom in to the window and look at the upper left side of the emblem.  The piece that belongs to polyline1 is not there!

This is the master template that I use for my data plate production, I simply change the verbiage at the bottom to reflect the data needed by the user.  Has worked just great for some time.

I even went an extra step and loaded in a couple of previously built files for data plates that have been made and shipped.  Every time I produced the "new" GCode, the emblem in each had the same piece missing on the left side.

Tomorrow morning I will continue with production on some new orders.  I am fortunate that I have a backup computer that is loaded with an earlier version that also has all the data plate information on it as well.  It is my backup production system, and I just did not get around to updating CamBam to the latest version.  Lucky for me huh!

I guess this is why it is called Beta Testing!

 Hopefully there is something that I have done incorrectly, but for the life of me I can't seem to find it.

Look forward to hearing back from you soon.

George
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on August 10, 2010, 08:21:45 am
The file was generated from DeskEngrave, a program I learned about  on this forum.  It generates text along a curve, something CB cannot do at this point.  I am attaching the file.

Thanks for that... the layer is indeed set to black.  I will put the layer color = background color check on the todo list.

You may also be interested in the fantastic Arc Text plugin that Hans_G created...
http://www.cambam.co.uk/forum/index.php?topic=348.0
(look toward the end of the thread to find the latest version)
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on August 10, 2010, 09:16:40 am
Hello George

Unknown Field/Property: MOPProfile._Tabs     When you acknowledge the error, the box closes and the highlighted text is erased.  Something is strange, but it does delete the object selected just fine.

This one is fixed now in the development version.

Quote
Now for the real problem that has stopped me in my tracks this afternoon.
...
The piece that belongs to polyline1 is not there!

Sorry about that...I will investigate to see what's going on.

In the mean time, I think it is easy to fix. In your profiles you have a tool diameter of 0.0001 set.
From memory, I think you said you were doing this to trick the profile into a doing a multi-depth level engraving operation (which 0.9.7 didn't do).

If you change the tool diameter to 0, this should have the same effect and seems to work OK. 

This should also be a lot faster and more reliable as CamBam is not trying to do an offset of 0.00005 which is getting very close to the math's tolerance limits... (which I think is what is causing the disappearing toolpath problem).

In 0.9.8 there is now also the option to do incremental depth engraving operations, however I just noticed that the engraving mop does not have a CutOrdering option to set DepthFirst, so the toolpath is not that efficient.
I have just added this which will be in the next release.

I hope that helps!
Title: Re: CamBam plus 0.9.8
Post by: GeorgeRace on August 10, 2010, 12:00:40 pm
Hi Andy:

As always, you have a solution to my situation!

Yes, using the profile MOP's really makes a nice looking "engraved" data plate.  When I use the engrave MOP I just can't seem to get the same results, and that seems strange to me.  Maybe as long as you have the file, you can tweak it a bit and make it work equally well using the engrave MOP's.  This plate takes about 40 minutes to make, due to the fact that each letter is done inside and out causing a double cut over the same path.  Maybe that is why it looks so good!  Kind of polishes the path the second time over in the opposite direction.  Incidentally I am using a 1/64 inch ball end mill to do the "engraving".

Making the tool diameter "0" brought back the tool path!  As usual you are FANTASTIC! ! !

In 9.7 the GCode was 11,931 lines in size, in 9.8 it is now 12409 lines.  Will give it a go this morning and see how it work out.

This is what BETA testing is all about!

Thanks, heading for the shop to make more scrap out of perfectly good metal!

George
Title: Re: CamBam plus 0.9.8
Post by: kvom on August 10, 2010, 21:34:45 pm
Are you saying that a profile MOP with a tool diameter of 0 is equivalent to an engraving MOP, but "better"?
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 11, 2010, 00:20:30 am
I created a new style library.
I created a new cam-style in it, named test.
I chosse a tool from the tool library an give in some values like target depth -10mm and depth increment 1mm.
From context menue I choose save to xml.
On the CAM Styles Folder with context menue I chosse refresh.
I draw a circle and chose a profile mop.

If I try to choose the "test-CAM-Style" CB tells me: "test not found"
If I choose then an other CAM-Style from the Standard-mm I don´t get the values from the template to the mop.
Then I deletet the CAM-Style "test" with context menue.

CB freezes. Nothing goes on
I close CamBam with ctrl+alt+del. 

After this I can´t restart CB.

I try delete the library "template.xml". At first windows tells me that some program use this file and I can´t delete it. After windows restart I can delete it and then CB works ok.


And some questions:

I try to understand how this CAM-Styles are working and how the styles interact with the other librarys like material and tools.
Perhaps it is possible that you can explain this when you have some minutes.
However, when creating new librarys or deleting CB reacts a bit huffy.

I found a speed and feed calculator. The calculator gets some values from the tool library, but not all, not the number of flutes, and not tooth load.

And what means "Add to active palette" when right klick a tool?

So many questions

ralf
Title: Re: CamBam plus 0.9.8
Post by: dwc on August 20, 2010, 06:02:37 am
Hi Andy,
I have been using 0.9.8 now for a while and am starting to understand some things.
Really only 2 things are bothering me right now:
1) when I apply a style to a MOP I have to leave the MOP and return for the inherited values to be shown correctly, it should happen immediately.
2) How about putting the CamBam version in the nc file header along with the date/time in international format, i.e. year.month.date-hours:minutes:seconds.  Then everyone will be equally happy or unhappy.

I tried to see how the feed calculator ties in to the styles yesterday, but then couldn't find it at all, although I know it has popped up at times.  Where have you hidden it? and can it automatically insert feeds if the material info, spindle speed and tool dia are known?

Keep up the great work!
Don

Title: Re: CamBam plus 0.9.8
Post by: Bench_Top_Precision on August 20, 2010, 16:32:48 pm
I think I may have found a bug in V0.9.8

I'm cutting a profile with holding tabs out of a piece of stock. The bug I think I came across is that once you select to use holding tabs for a profile MOP and then want to select more geometry for another MOP it thinks you are trying to drag the holding tabs every time you click and effectively setting your "Auto" to "Manual."

I even tried to disable the MOP and it still does it. Nothing major I just set the holding tabs for that particular MOP to "None," select what I need to and then re-enable the tabs to "Auto" or "Manual."

~Scott
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 20, 2010, 20:19:07 pm
If you have any property set to auto and then you insert a value, it switch the setting from automatic to manual.
That is not a bug, cause you set a value manual and so it has to change the property from auto to manual.

The thame thing with the tabs. If you generate tabs, you generate a tab-collection, it is like a point list.
It is a list with the coordinates of the tab. You can open the collection bei clicking the [...]-Button.
So, if you change a tab bei clicking on it, you change only the coordinates in the tab-collection and it is a manual action. So CB change the property to manual. You can change the coordinates of the tab also in the tab-collection.


ralf

Title: Re: CamBam plus 0.9.8
Post by: EAC on August 20, 2010, 21:58:34 pm
Found another problem with 0.9.8...

The Tab Height is measuring from the wrong place.  It should, as it did in .9.7, measure the height from the Target Depth, so you get an accurate height of the tab.  It now measures the Tab Height from the clearance height.

Don
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 20, 2010, 23:02:24 pm
Don.
Are you sure it isn't referencing the Style setting?

Martin.
Title: Re: CamBam plus 0.9.8
Post by: dwc on August 21, 2010, 06:23:39 am
Found another problem with 0.9.8...

Will have to check that out.  I have done a rather complicated part with tabs with 9.8. and it looked OK, but haven't triet to cut it yet.  Thanks for the tip.
Don
Title: Rotate Seems Strange
Post by: GeorgeRace on August 21, 2010, 12:21:48 pm
Hi Andy:

As an example, I draw a rectangle.  I then select Edit/Transform/Rotate

The mouse and the small green square, that is the rotate position indicator, are not together at all.  One seems to be going the opposite way of the other.  If I move the mouse pointer to the far right on my screen, the small green square starts to come in from the left side of the screen, several inches apart.

Is this me, or might there be some kind of a glitch in CamBam?

George
Title: Re: CamBam plus 0.9.8
Post by: EAC on August 21, 2010, 14:40:40 pm
Found the issue with the tab height.  Have to watch the warning box.  In 97, if you put in a positive target depth, it changed the target depth to stock surface, so it basically cut on the zero level, and you noticed your mistake when you rotated the drawing.

In 98, if you put in positive target depth, it says it changes it to "-" target depth. It now cuts right with the wrong input, but apparently doesn't re-reference the tab height to the new target depth, so the tabs are the wrong height.

Finding this kind of stuff is what beta testing is all about  ;)

Andy, I think a better fix to this would be to set the target depth property to only allow negative input, that way the user can't put in a positive value.  I think you can do that.

Don


Don.
Are you sure it isn't referencing the Style setting?

Martin.
Title: Re: CamBam plus 0.9.8
Post by: rezcar on August 21, 2010, 16:50:22 pm
I think Scott was trying to select another piece of geometry nearby but CB thinks he's trying to select the tab, and changes it to "manual". Happens to me all the time. I just started using Viacad and if objects are stacked or grouped closely together, it asks you which object you want to select. And you can confirm which object as Viacad hightlights it as you drag your mouse down the list.

If you have any property set to auto and then you insert a value, it switch the setting from automatic to manual.
That is not a bug, cause you set a value manual and so it has to change the property from auto to manual.

The thame thing with the tabs. If you generate tabs, you generate a tab-collection, it is like a point list.
It is a list with the coordinates of the tab. You can open the collection bei clicking the [...]-Button.
So, if you change a tab bei clicking on it, you change only the coordinates in the tab-collection and it is a manual action. So CB change the property to manual. You can change the coordinates of the tab also in the tab-collection.


ralf


Title: Re: CamBam plus 0.9.8 minor bugs
Post by: airnocker on August 21, 2010, 21:24:31 pm
Hi,

Just started playing around with 0.9.8.  I like it and the improvements you have made.

I found two minor bugs.

The html Help file incorrectly points to where the Sample files are.  It currently points to here:
file:///C:/Program%20Files/CamBam%20plus%200.9.8/help/samples/heart-shaped-box.cb but "/help" should be omitted from the path.

When setting the Text font size, anything smaller that "1" generates an error shown in the attached jpg file.

airnocker

Title: CamBam computer lockup adding (-) sign to depth field
Post by: GeorgeRace on August 21, 2010, 23:45:42 pm
Hi Andy:

Just a heads up in case this may be happening to anyone else.

I was setting up a drilling MOP from a points list.  I failed to put a (-) sign in front of the cut depth.  When I went back and put in the minus sign, the computer went into a waiting loop and the only way out was to reboot the computer.

So, I came into my office and tried the same operation on another machine.  Did exactly the same thing and had to reboot to get back in operation.

Now, have tried to recreate the same thing again and no matter what I do CamBam just sets there doing everything it should just fine with no lockup.

If I can figure out what I was doing differently I will try to save the file and forward it on.

George
Title: Computer Lockup with Drilling MOP
Post by: GeorgeRace on August 22, 2010, 13:39:20 pm
As I reported last evening, I was getting a lockup of the computer during entry of a Drilling MOP.
This morning I went back to the project and NOW have documented what I am doing to cause the lockup of the computer.  It happens on three different computers here so I think it may be a CamBam problem.

Will someone please do the following steps and let me know if this is happening to you as well.

Load in my attached file:  Dennis 701 Side Access Panel.cb
Select Point List (45)
Click on the "Drill" icon in the top row

Now fill in the following areas of the Drill MOP. (I delete the default item first, then add the new value)

Name  Drill Outer Holes
DepthIncrement   0.0
TargetDepth    -0.055
DrillingMethod    SpiralMill_CW
HoleDiameter    0.125

As soon as I hit the Enter Key, after typing in 0.125, the computer locks up and a reboot is necessary to get running again.

This Drill MOP, with the same parameters, is being used in a lot of other operations that I am doing and were made with the previous version of CamBam.  They all are working just find and can be loaded and run in CamBam Plus with no problem.  I can even go in and make changes without anything going wrong. 

I just can't seem to enter a NEW Drill MOP without the computer locking up.

Help Please!
George
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 22, 2010, 14:47:41 pm
Sorry GeorgeRace,
I can´t confirm this.
I take your file, attach a drill MOP to pointlist45, give them your values and I can generate the toolpath.
No problems with the file.
 
Title: Re: CamBam plus 0.9.8
Post by: Bertram on August 22, 2010, 15:36:16 pm
George, I tried your numbers and the programme locked on me too. Change the Depth Increment value to something other than 0.0. A DepthIncrement of 0 will have the cutter spiralling endlessly at the top of the stock and not actually boring down into the material.

PixelMaker, yours worked because you didn't change the DrillingMethod to SpiralMill_CW.
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 22, 2010, 15:55:12 pm
It locked up for me too, but if I used ralf's file and entered the right numbers it worked OK  ???.
I copied this from the What's New documentation:- Changes to drilling

A DepthIncrement property has been added. This is now used to calculate the pitch for spiral drilling methods. If depth increment is 0, the old method of using the ratio of the plunge and cutting feedrates will be used.

So it looks like it's designed to work in this way (but without the bug).

Martin.
Title: Re: CamBam plus 0.9.8
Post by: Bertram on August 22, 2010, 17:24:40 pm
George, what size tool are you using to drill the holes?

When I generated my numbers, I used the default 0.093 for the tool diameter and a spiral was generated.

PixelMaker appears to have used 0.125, another reason we are getting different results.
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 22, 2010, 18:14:57 pm
I don´t use a spiral drill. I my file it is a canned cycle.
It was my mistake.

When I give SpiralMill CW without a DephtIncrement, CB gets very slow.
After 5 minutes I can generate toolpath and then I get an "out of memory" prompt. I hit ok and CB things again some minutes.When I give CB then a DepthIncrement it works as fast as normal.

I try it more times and it is always the same, when I give  a DepthIncrement before I give the value TargetDepth there is no problem.
When I try to give TargetDepth befor DepthIncrement the problem occures.

So GeorgeRace, please give him a DepthIncrement and then we can wait for 10B
And the hole diameter must be larger then the tool.




Title: Re: CamBam plus 0.9.8
Post by: GeorgeRace on August 22, 2010, 23:58:39 pm
George, what size tool are you using to drill the holes?

When I generated my numbers, I used the default 0.093 for the tool diameter and a spiral was generated.

PixelMaker appears to have used 0.125, another reason we are getting different results.

My bit size is .093.  During the process I do several different MOP's.  Some require a .24 diameter hole, others require a .125 hole, and there there are several that are just "Drilled" with the .093 mill giving me a 1/32 size rivet hole.

The reason I used Zero for the depth increment was due to the fact that it said to do that with the new CamBam, as was pointed out by blowlamp back up the list.

I added a depthincrement and got it all working later on this afternoon.

The whole point of this discussion is to simply point out a programmatic error.  There should not be any circumstances that with a wrong input value cause a computer program to hang up.  A pop up message reporting the error would be more appropriate.

I am sure that Andy will find and eradicate all of these kind of bugs.  That is why this is called BETA TESTING, to find and clear up anything that is not working correctly.
Thanks to all for your comments, greatly appreciated.
George
Title: Re: CamBam plus 0.9.8
Post by: rezcar on August 23, 2010, 02:09:41 am
Cut my first part with 0.9.8 today, it had 3 MOPS using 0.125, 0.375, and 0.375 tool diameters in that order. It never stopped and asked for a tool change, just kept right on cutting.
Title: Re: CamBam plus 0.9.8
Post by: Bench_Top_Precision on August 23, 2010, 11:28:31 am
Quote
Cut my first part with 0.9.8 today, it had 3 MOPS using 0.125, 0.375, and 0.375 tool diameters in that order. It never stopped and asked for a tool change, just kept right on cutting.

Did you check to see if there were M6's in the G-Code?

~Scott
Title: Re: CamBam plus 0.9.8
Post by: dwc on August 23, 2010, 12:39:14 pm
Cut my first part with 0.9.8 today, it had 3 MOPS using 0.125, 0.375, and 0.375 tool diameters in that order. It never stopped and asked for a tool change, just kept right on cutting.

Did you give each tool a different tool number ?
CB does not look at the tool size defined to determine when to change tools.
It changes tools when it sees a differrent tool number.
The tool size is used for defining the tool path.
0.9.8 has been working correctly for me in this regard.
Don
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 23, 2010, 15:46:03 pm
It would be convenient if the previous behaviour of ToolDiameter could be retained, for people like me that regrind their cutters to odd sizes and can't be bothered with formally defining them. That is to say, I think that in the absence of a ToolNumber, CamBam should look for a ToolDiameter and act accordingly.

Martin.
Title: Re: CamBam plus 0.9.8- the performance
Post by: pixelmaker on August 24, 2010, 00:09:28 am
Today I played  with the new behavior for making a heightmap from a 3D surface with the ->Draw ->Surface->From Bitmap.
It works fine.
But I need very long time to generate the toolpath. When I set the Profil3DMethod to Horizontal and RegionFillStyle to HorizontalHatch, it needs about 8 min for rendering the toolpathes for a 2mm tool, in a heightmap with a height from 200mm and a StepOver from 0.4. (The green-man-bw.jpg).
With other Profil3DMethods and RegionFillStyles it needs up to 1 hour.

What I wonder is, that CamBam the hole time only works with one of my eight processors. Is it possible, that CamBam is not capable to work with multi processors ?
Or is this a thing of my computer?
Title: Re: CamBam plus 0.9.8
Post by: dave benson on August 24, 2010, 02:26:38 am
HI All
I've been slowly migrating my 07 files to 08 and and have hit a snag with the drilling mop.
In 07 there is a property DepthRelaitveTo -->StockSurface,absolute,Geometry
Which i have set to --> Stock Surface.
And i can't find this Ability  in 08.
Attached is a 07 file that works, So that you can see what I'm trying to achieve with 08.

Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 24, 2010, 10:42:57 am
hello dave,

in the help documents you can find under "Changes to drilling":
TargetDepth is now specified as an absolute Z coordinate, to make it consistent with all other machining operations. In previous versions target depth was a relative offset from the stock surface.


ralf
Title: Re: CamBam plus 0.9.8
Post by: dave benson on August 24, 2010, 11:50:29 am
Thanks Ralf
Sheezzz When all else fails read the manual!
I appreciate (the keeping things consistent methodology)  however this means I'll have to use 07 for this job
as that file was one of 3 (spot face,centredrill and deep hole drill)So thats 135 manual edits to the z depth. :o
Title: Re: CamBam plus 0.9.8- the performance
Post by: blowlamp on August 24, 2010, 12:01:24 pm
Today I played  with the new behavior for making a heightmap from a 3D surface with the ->Draw ->Surface->From Bitmap.
It works fine.
But I need very long time to generate the toolpath. When I set the Profil3DMethod to Horizontal and RegionFillStyle to HorizontalHatch, it needs about 8 min for rendering the toolpathes for a 2mm tool, in a heightmap with a height from 200mm and a StepOver from 0.4. (The green-man-bw.jpg).
With other Profil3DMethods and RegionFillStyles it needs up to 1 hour.

What I wonder is, that CamBam the hole time only works with one of my eight processors. Is it possible, that CamBam is not capable to work with multi processors ?
Or is this a thing of my computer?

ralf.

Have you yet set the Worker Threads to = how many cores your computer has, under Options in CamBam?

Martin.
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 24, 2010, 14:26:36 pm
Oh wow,
I ever think the Worker Threads means how many guys are disputing in front of the computer and the value is measured in bottles of beer.

It reduce the rendering time a lot. With a bitmap (the green man) and a Grid Stepover of 0.1 and a tool from 1mm with StepOver from 0.1 it needs now only 5 minutes.
Thank you a lot

ralf
Title: Re: CamBam plus 0.9.8
Post by: Bench_Top_Precision on August 24, 2010, 14:57:22 pm
I'm having some issues with the pocketing step over.

What's happening is, I'm cutting a pocket with a Ø3/8 endmill and using a spiral ramp lead in.

I did a little testing (see pictures). The first picture is a 69% step over, as you can see indicated by the blue line, after it spiral ramps to the desired depth it then has a linear move to the next step over (blue line) which is what I want.

The next picture is 70% step over and this appears that it only will do the linear step over on the last one.

The last picture is 71% step over and will not do any linear moves. It does the first spiral ramp into the part then makes the cut at that depth, rapids out, and over to the next, then repeats.

This proposes a problem for me because I like to use 75% step over. Is it a bug?


~Scott
 
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 24, 2010, 15:36:10 pm
Scott.
Have a fiddle with the MaxCrossoverDistance and see if anything changes.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: Bench_Top_Precision on August 24, 2010, 17:14:57 pm
Yep that did it. I didn't see that function. Not sure when you would need to limit how far it will step over but I just set it to 1.0 and everything is normal.

It was set at .7 by default which makes perfect sense why any value over 70% wouldn't do a linear step over.

Thanks man,

~Scott
Title: Re: CamBam plus 0.9.8
Post by: dwc on August 24, 2010, 17:49:01 pm
Not sure when you would need to limit how far it will step over

At least for me it works wonderfully when I want to force a rapid up at the end and a new spiral in for each path.

Don
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 27, 2010, 09:05:34 am
CamBam 0.9.8 won't open today :'(.
I've had a Windows 7 update on the computer and I'm wondering if this is the problem. Reinstalling doesn't help. Is anyone else having the same trouble?

Martin.
Title: Re: CamBam plus 0.9.8
Post by: Bench_Top_Precision on August 27, 2010, 09:19:17 am
No problem here. I'm in XP though.

Although one thing I noticed is that If I try to open a .cb file from this website. E.G. I download and choose to open it from my web browser, CamBam thinks I'm still using an evaluation and doesn't recognize that I have a license.

But if I open CamBam first, then open the .cb file, everything is fine.

Kinda weird, but just doing my part to help CamBam be the best it can be.

~Scott

Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 27, 2010, 10:53:20 am
Scott.
I think it's doing that because Andy hasn't set up the 0.9.8 'unproven release', to associate to .cb files yet.

I hope you're finding CamBam good to use alongside BobCAD/CAM.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: EAC on August 27, 2010, 14:03:27 pm
No problems here on W7...  The only startup problems I had was after deleting the un-named (blank) CAM style, that was early on before we found out not to delete it.  Had to uninstall and reload to fix it then.

Don

CamBam 0.9.8 won't open today :'(.
I've had a Windows 7 update on the computer and I'm wondering if this is the problem. Reinstalling doesn't help. Is anyone else having the same trouble?

Martin.
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on August 27, 2010, 18:13:50 pm
CamBam 0.9.8 won't open today :'(.
I've had a Windows 7 update on the computer and I'm wondering if this is the problem. Reinstalling doesn't help. Is anyone else having the same trouble?

Any joy with this yet Martin?
I've seen similar problems when style libraries get corrupted.  Look in the
Documents and Settings\All Users\Application Data\CamBam plus 0.9.8\styles
folder (or rather the Windows 7 equivilent) and look for any zero length .xml files and delete them.
Title: Re: CamBam plus 0.9.8
Post by: spiked3 on August 27, 2010, 19:19:44 pm
Curious; what is the suggested methodology on tool change and height?
I am using a fast plunge now. It executes it before the tool change. In the normal course of action I jog higher, change tool, reset Z with a setter (so that its usually around 1" when Im done) and hit go.  Since we've already done the tool plunge line of code, I wait while it slowly descends over an inch.
I haven't toyed with the 'tool change' height in Mach3 - and maybe that's the right thing to use, but it seems like it would only move to that height, not move from it before it resumes?
Otherwise, I guess I could edit the macros and add a plunge after the tool change - if that is the case, shouldn't this be the default - wouldn't most people want this to happen after?
So, again, just curious what the 'best practice' is in the wild.

Mike
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 27, 2010, 19:42:27 pm
All sorted now chaps, thank you.
I uninstalled 0.9.8 with Revo to get rid of as much junk as possible, but when I reinstalled I got an Incorrect Install message, from Windows. Redoing with Full Admin Control seemed to fix it in the end though. Never had to do that before, so something's changed recently.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 27, 2010, 21:11:16 pm
Please, I could not find the Machining Option ToolpathVisibility -> SelectedOnly in 0.98.
Don´t exist this option not any longer in 0.98?

Thanks

ralf
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 27, 2010, 22:01:39 pm
ralf.
Here you go.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: Bench_Top_Precision on August 28, 2010, 13:58:07 pm
Quote
Scott.
I think it's doing that because Andy hasn't set up the 0.9.8 'unproven release', to associate to .cb files yet.

I hope you're finding CamBam good to use alongside BobCAD/CAM.

Martin.

Martin, I haven't opened BobCAD since I bought my CamBam license.  :)

~Scott
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on August 28, 2010, 15:15:11 pm
Aaaah thank you martin

ralf
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on August 29, 2010, 12:26:11 pm
Quote
Scott.
I think it's doing that because Andy hasn't set up the 0.9.8 'unproven release', to associate to .cb files yet.

I hope you're finding CamBam good to use alongside BobCAD/CAM.

Martin.

Martin, I haven't opened BobCAD since I bought my CamBam license.  :)

~Scott

Andy.
There's one for your Quotable Quotes Section  ;)

Scott.
Wow, that's a surprise, 'cos I know BobCAD/CAM has come on a lot recently!
Can you use its CAD section to export DXF and STL files to CamBam OK?

Martin.
Title: Re: CamBam plus 0.9.8
Post by: kvom on August 29, 2010, 12:51:15 pm
Quote
Can you use its CAD section to export DXF and STL files to CamBam OK?
That's what I do when I need some more complex drawing than CB provides.
Title: Re: CamBam plus 0.9.8
Post by: Bench_Top_Precision on August 29, 2010, 13:05:53 pm
Quote
Can you use its CAD section to export DXF and STL files to CamBam OK?

You can, I don't. Drawing in BobCAD is a bit quirky. I use SolidWorks for all my CAD and 3D modeling work.

I never would have bought BobCAD if it weren't for the ridiculously low price ($300) the salesman gave me.

I want to try some 3D work with CamBam soon. I know awhile back there was an issue with the Waterline MOP. I assume this was fixed.

~Scott
Title: Re: CamBam plus 0.9.8
Post by: Bubba on August 29, 2010, 23:28:53 pm
"I know awhile back there was an issue with the Waterline MOP. I assume this was fixed."

As long you use the "Level First" for your depth settings , you go to go! 8)
Title: I did it again - documentation 0.9.8 in german
Post by: pixelmaker on September 03, 2010, 01:53:09 am
I finished the german translation of the documentation for 0.9.8 in german.
Unfortunately  it is to big for uploading in the forum.
I place it on my server for  downloading.
Perhaps 10bulls can place it somewhere.
Here is the download (9.1Mb) (http://pixelmaker.eu/cambam/dokumentation_german_CamBam_0.9.8.zip)

Title: Custom Drill Scripts in 0.9.8
Post by: dwc on September 03, 2010, 06:54:07 am
Hi Andy,
I discovered this morning that it is not possible to define a custom drill script in a style in 0.9.8
I can, however, define the custom drill script in the MOP, so it is not a show stopper, but a pain.

In details, the window to define a multiple line custom drill script is not available when defining the style.
I tried to define a one line custom script in a style, but it is not taken into consideration when the MOP is produced.
The code produced in that case is just a position to the first hole.
The code produced from a custom script defined in a MOP appears at first glance to be OK, but I haven't checked it in detail.

It would also be nice if the [ ] from g-code expressions didn't cause an error message, but again we have been living perfectly well with the error message up 'til now. :)
Don

Title: Re: I did it again - documentation 0.9.8 in german
Post by: 10bulls on September 03, 2010, 11:08:11 am
I finished the german translation of the documentation for 0.9.8 in german.
Wow!  Once again, I can't thank you too much for that and I am sure it will be greatly appreciated.

Website changes will be soon now so I will be sure to put a link to your documentation there.

Thank you once again!
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on September 03, 2010, 22:30:06 pm
 You're welcome!
With my poor english and with no internet and a small laptop screen at my machine, it is more easy to have the documentation in a book and in german also.
What I forget is an index with keywords, this I have to do next.
And for sure I also do the english book.

Some questions I have now about CamBam.
1. In cam-styles it is not possible to choose a tool from the tool library. Although I can select a toolnumber, but the tool profile and the diameter dont come from the library. I have to write it.

2. Is there any language file in CamBam, like a xml-file where I can translate Cambam itself to german?
Or make it sense to create a database with the translation of the menus to  to help you get a german UI?

ralf
Title: Re: CamBam plus 0.9.8
Post by: Desertrunner on October 02, 2010, 05:47:56 am
Well had to bite the bullet and give 9.8 a go and I love it,  worked brillantly, saved me heaps of time on setup and also milling time.  Its going to take a while to get my head around.  Did have one small problem the program below didn't mill with tabs.  I think it maybe my fault because I just realized the tab width was set at 1.5 mm not my normal 5mm.
Tony
Title: Re: CamBam plus 0.9.8
Post by: Desertrunner on October 02, 2010, 08:03:33 am
Just figure it out, you smart buggar 10bulls, I increased the width and the height because the tag are ramped on and off of.

Love the new version it brillant
Tony
Title: Re: CamBam plus 0.9.8
Post by: mhackney on October 07, 2010, 23:34:05 pm
Very cool! I've been using CamBam for about a 9 months now with my mill. I just acquired a cnc'd Sherline lathe and need software. So I thought I'd check and see if CamBam supports lathe - just to discover the new beta version does! So, rather than spend my time and money on another product, I'll pitch in and test CamBam and provide my feedback.

I also like the new Part mechanism. This will help me a lot as will Materials and Tools specifications. Great job!

cheers,
Michael
Title: Re: CamBam plus 0.9.8
Post by: pietvr on October 08, 2010, 03:21:31 am
Hi

There might be some technical improvements but I am  :( sad to say, instead of making your GUI more user friendly, it seems like you made it more complicated. ??? Selectig MOP's has become an even bigger "shlepp" with this new version.

I will keep working with Version 0.9.7F untill there are real improvements to MOP selection in the GUI as well.

Why not make the toolbar customizable so buttons can be added by users, for eg. "Zoom To Fit"?

Cheers

Piet

Title: Re: CamBam plus 0.9.8
Post by: blowlamp on October 08, 2010, 07:37:53 am
Hi pietvr.
What's a "shlepp"?

Martin.
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on October 08, 2010, 09:14:14 am
Thank you everyone for the comments and suggestions.

Piet - When you say "improvements to MOP selection in the GUI as well", do you mean being
able to select MOPs by clicking objects in the drawing window?
I am considering this for future releases.  One way would be to detect clicking on toolpaths in the drawing view then select the associated machining operations.  Would this be of help to you?

I didn't think MOP selection was much more trouble in 0.9.8.  True there is the extra 'Part' level now, but personally I have found this makes it a lot easier to organise and locate MOPs, especially with complicated drawings.  I did consider hiding the Part folder in the tree if there was only one part (so it would appear the same as 0.9.7), but figured this would add unnecessary complexity. 

Michael - I would very much appreciate any feedback on the lathe operations.  I should reiterate the warnings in the release notes - it's very new and experimental, could be made more user friendly, wear safety helmets and ballistic pants etc etc.  But with testing and suggestions for improvement I am sure it can soon be knocked into shape.
Title: Re: CamBam plus 0.9.8
Post by: mhackney on October 08, 2010, 11:08:18 am
The Sherline lathe I acquired is in a cabinet with a thick lexan clamshell panel! I'll be mostly machining Delrin on this machine too. I always preflight my gcode "dry" before cutting a part too. I tend to be a little over cautious as well. Thanks for the warning!

Cheers,
Michael
Title: Re: CamBam plus 0.9.8
Post by: Desertrunner on October 08, 2010, 18:46:07 pm
Piet,
I want to jump in here as I beleive I have to disagree with you.
When I down loaded the 9.8 I took one look and decided it was to complicate so I would skip upgrading.  Last week the old version caused a cutter to dive and I broke 2 of them before I realized there was a floor in the code.  I needed to get the job done so I had to upgrade.  Now I am in Love, I will never in a million years go back to the old version, no way not ever.  I was blown away by how much faster the new one was to program and I beleive it cut my mill time down to a third of what it was before.
So I ask, beg and what ever else I need to do to get you to do one trial for me.  I want you to cut out a circle plate.
Open version 9.8 and go to "System" tab up the top then double click "Cam Style", click either "Standard-in or metric.
Select "cutout+tabs" you should see the MOP appear below.  Were the four buttons are chose the one on the far left next to the A-Z one.  That way your layout will be the same as the old version.  Go down and set the parameter as you would normaly.  As you are in the holding tap version you will need to adjust them as well in metric I run 4 mm high by 6mm  wide.  I set speeds depth increments even maxium depth and tool size all in this set up (I cut mostly 10mm plate).  When you are finished close the program and restart it.  This saves your templets.
Okay reopen the program draw a shape you want to cut out, high light it, then pick profile.  Look down the list of set up (5th line) Style and slect "cutout+tabs", after that you need to click oin the work area to activate the new templete. Set any other setup you want, down load the code then give it a go on your mill.
After that if you still think the old version is better I will be happen to accept it.  The new version is so fast you will never go back.
Have a great day.
Tony
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on October 13, 2010, 23:41:54 pm
It looks that Desertrunner found a bug with Stepover:
http://www.cambam.co.uk/forum/index.php?topic=1302.0

If I set the DepthIncrement in the 3D-profile of his cb-file to 0 the Stepover is correct. If I set DepthIncrement >0 the StepOver is only the half of the fraction of the tool-diameter.
Title: Re: CamBam plus 0.9.8
Post by: Desertrunner on October 14, 2010, 20:14:16 pm
As mentioned the height is wrong by the width of the cutter, if this turns out to be a bug is it possiable that this problem is causing the error when you cut "Depth First"
Tony
Title: Re: CamBam plus 0.9.8 dxf export
Post by: pixelmaker on October 14, 2010, 21:36:40 pm
today I make a 3D-surface from a foto with the new -> draw -> surface -> From Bitmap function.
Then I try to export the surface to dxf.
The dxf is empty. When I open it with autocad ther is no object in it. The filesize is only 4kb.
Title: Re: CamBam plus 0.9.8
Post by: Bench_Top_Precision on October 16, 2010, 01:10:46 am
Don't quote me on this but I don't think you can create an actual DXF from a height map. It only produces a tool path to cut and not an actual part.

10bulls would be the man to ask on this one.

~Scott
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on December 18, 2010, 12:09:26 pm
Can the Toolpath index and the Z depth index in the new Toolpath View Filter, be made to display the first cut at 1 rather than 0? I find it a bit unintuitive when tracking through the toolpaths. As a non-mathematcal type, I struggle with the concept of something happening when I have a zero before me.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on December 18, 2010, 17:58:23 pm
I'm trying to add a tool to the Default-mm folder, only when I come to save it, I get the error message 'Access to the path is denied'. I can save tools elsewhere without problem, but wondered why the Default folder can't be added to.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on December 20, 2010, 01:23:23 am
I'm trying to add a tool to the Default-mm folder, only when I come to save it, I get the error message 'Access to the path is denied'. I can save tools elsewhere without problem, but wondered why the Default folder can't be added to.

Ah yes, I wondered how much of a problem this would be.

The easy 'fix' is to go 'Tool - Browse system folder', then in Windows Explorer, go up a level and do right click, properties on the 'CamBam plus 0.9.8' folder.  Now in the Security tab, give your user account 'Full Control' permissions.

Alternatively, in CamBam's system configuration settings, you can change the SystemPath property to point to your user profile folder... 
{$user}\CamBam plus 0.9.8\
...or an alternative location.

From a security, best practices point of view I should perhaps make the user profile the default location for the system folder.  Personally though, I prefer the common application area.  Especially if installing on a machine with multiple users.


Title: Re: CamBam plus 0.9.8
Post by: EAC on December 20, 2010, 04:05:47 am
Andy, found an issue with the new 'post' system.  The new system works great, until you load an older .CB file.  The old .cb file doesn't know about the new posts, so if you save a g-code file, your post changes aren't applied.  Bad things can happen  :o

If an older .cb file is loaded, you need to automatically set the post to the post called in your template file, so it will be used when creating g-code, and saved in the .cb file when it is saved as the new version.

Don @ EAC
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on December 20, 2010, 21:53:52 pm
Hi Don,

Is this the same problem as in this post?...

http://www.cambam.co.uk/forum/index.php?topic=1411.0

Sorry for moving the location of the post files on you but I thought it best to keep 0.9.8 separate to 0.9.7.

Andy, found an issue with the new 'post' system.  The new system works great, until you load an older .CB file.  The old .cb file doesn't know about the new posts, so if you save a g-code file, your post changes aren't applied.  Bad things can happen  :o

If an older .cb file is loaded, you need to automatically set the post to the post called in your template file, so it will be used when creating g-code, and saved in the .cb file when it is saved as the new version.

Don @ EAC
Title: Re: CamBam plus 0.9.8
Post by: EAC on December 20, 2010, 22:58:18 pm
Completely different problem.  Only occurs when loading a pre-.98 .CB file.  Everything works perfectly on new files, and .98 .CB files.

Everything else converts and works, i.e: all the MOP settings.

What it doesn't reads the post that was used when the file was created. That could be 3 years or so old. If the name isn't found, It uses a default un-modified post.  That can cause some problems if there are important things in the post you are using. 

Can be worked around, but easy to forget to change to new post before creating G-code.  It may be because the names of my post have changed slightly as time goes on. 

For safety issues, I would thing that old files would be set to use current default post, the one that is loaded in the template file.  Also, as time goes by, things are added to post files to make them better for your use, ot changes in your CNC machine, making the old ones obsolete. If not changed to the current post, at least give an error dialog stating that the post in the .CB file doesn't exist, and a default will be used, so we know to change it.

Does that all make sense?

Don




Hi Don,

Is this the same problem as in this post?...

http://www.cambam.co.uk/forum/index.php?topic=1411.0

Sorry for moving the location of the post files on you but I thought it best to keep 0.9.8 separate to 0.9.7.

Andy, found an issue with the new 'post' system.  The new system works great, until you load an older .CB file.  The old .cb file doesn't know about the new posts, so if you save a g-code file, your post changes aren't applied.  Bad things can happen  :o

If an older .cb file is loaded, you need to automatically set the post to the post called in your template file, so it will be used when creating g-code, and saved in the .cb file when it is saved as the new version.

Don @ EAC
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on December 21, 2010, 10:10:49 am
Does that all make sense?

Yes, I think as you suggest a warning message should be added if the post is not found.

I was also thinking of adding a default post processor option to the Tool - Options settings.  So you could still set it in your drawing template, but if this was blank it would use the default system one.

Thanks Don!
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on December 21, 2010, 17:00:11 pm
I just noticed that Climb and Conventional milling strategies look like they're mixed up if I have OptimisationMode set to None when cutting a pocket.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on December 21, 2010, 20:32:36 pm
Ah, I see what you mean.

The toolpaths are in the same cut direction as the optimised ones but because they are output in the order they were generated they are going outside in, rather than inside out as the optimised ones do.

I think the toolpath order just needs to be reveresed when OptimisationMode=None is used.
I looks like 0.9.7 was doing this OK.  :(
I'll put this on the fix list.

Thanks Martin
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on December 21, 2010, 20:58:39 pm
Andy.
Does that mean that the cut then will start in the centre and work its way out to the edge, because I was trying to force an outside to inside strategy for this job?
I would like to remove all the outside stock from this part without doing any plunge cuts if possible and the ability to change to an 'outside inwards' strategy would be nice for doing this.
I'm finding the new Stock and Part features to be very nice  8) thanks!

Martin.
Title: Tab question
Post by: mhackney on December 28, 2010, 02:27:33 am
I have a round part and wanted to add 3 tabs. I set up the tab parameters as manual and min=2 max=3. When I generated the machine code, no tabs appeared. I then set tab to auto and regenerated. Now I get 4 tabs!  I can't seem to get the 3 tabs I want and I don't understand how manual works.

Cheers,
Michael
Title: Re: CamBam plus 0.9.8
Post by: dh42 on December 28, 2010, 15:32:39 pm
Hello

You can add or remove tabs by following this steep

- select the MOP that have tabs
- on the drawing right-clic on a tabs you want to delete and select "Holding Tabs/remove tab" in the context menu

You can change placement of tabs by clic and drag it with mouse.

Same think to add a tab -> "Holding Tabs/add tab" in the context menu

for automaticaly obtain 3 tabs, you can try to set min and max tab to 3 and then use "Holding Tabs/autocalc" in the context menu to refresh the tabs (or setting "TabMethod" to Auto and generate toolpath again)

++
David
Title: Re: CamBam plus 0.9.8
Post by: mhackney on December 29, 2010, 01:24:52 am
Thanks David. That did the trick.

Regards,
Michael
Title: Re: CamBam plus 0.9.8
Post by: Gneyenhuis on December 30, 2010, 05:55:09 am
I have used 6 of my trial starts of CamBam Plus. I have been using 9.8 g & h til now. I just got my cnc router finished a couple weeks ago so I'm new. Today I was engraving a pattern of squares app 3/4 in. layed out like a single array of 15 squares. Each of these have a smaller square inside of it and each of them has a smaller square inside of it and each of them has a still smaller square inside of it. I hope this explains my pattern. When I produce the tool path it put in cuts between some of these squares - either vertical or diagonal. Looking for the solution, I downloaded the newest stable release and it produce a correct tool path. Ive spent the last 10 months designing and building my machine and so I've been looking at all the CAM programs available and I am sold on CamBam. My plan is to build jewelry boxes with very small patterns and engravings on them. I will keep playing with the latest editions because I'm still learning - and I really like the new features you are adding. Very COOL intuitive program.
Thanks
Gary N.
Phoenix, AZ, USA
Title: Re: CamBam plus 0.9.8
Post by: lloydsp on December 30, 2010, 13:51:35 pm
Gary, I'd been using G-simple for most of two years on my restored R2E4.

A friend recommended CAMBAM.  After using it about ten days, I purchased it. 

GSimple was free.  CamBam is a better deal!   ;D

LLoyd
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on December 30, 2010, 20:43:24 pm
I'm wondering if the Toolpath View Filter is working as intended. In short, I don't think things are being displayed in the order they perhaps should be for maximum effect. I mean, shouldn't the Profile MOP be shown in its entirety (in Toolpath index mode) before showing any of the Pocket MOP, so you can follow each toolpath start to finish?
I hope the video explains my point.

File courtesy of dh42  :)

Martin.

http://www.screencast.com/users/Hammering/folders/Jing/media/99fc6647-8459-4ff8-9b3f-eb0a3daff96f
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on December 30, 2010, 20:46:59 pm
If I understand the problem, I think you can do this if you set the toolpath view mode to 'selected toolpath only', under the top level drawing properties.  You should then be able to select a mop in the tree and step through just the toolpaths for that operation.

Title: Re: CamBam plus 0.9.8
Post by: bikegeek on January 03, 2011, 01:48:53 am
The default for Spindle Direction in the provided styles, IMO, should be CW.  The first g-code I generated with 0.9.8 had no M3 code.

I agree with you...but I can't seem to replicate this one.
The default spindle direction should be CW and the default spindle speed should be 1000.
I am not sure why you aren't getting an M3 in your post.... If you have a .cb file, I can check this out.

Sorry to jump in late on this post, but I seem to be having a similar problem: when I generate my gcode, I get an M3 line without any spindle speed controls. 

In 0.9.7f, I would get the line:
M3 S1000
in 0.9.8h, I just get:
M3

In the interim, I've been producing my gcode, then editing it.

I can send you a simple .cb file if you want.
Title: Re: CamBam plus 0.9.8
Post by: rezcar on January 03, 2011, 04:29:26 am
Trying to get my head around the tools functions in the new release. Hopefully this makes some sense.

In the "Default-Inches" library, changing a tool's property, index, etc changes the description automatically. It doesn't do it with libraries I created. It's frustrating to have to re-enter my custom description if I am changing something about the tool.

If I have 3 tools (what's the max number by the way?),
#1 3/8 2 flute ball
#2 3/8 2 flute endmill
#3 3/8 4 flute endmill roughing

and I bought a new 3/8 3 flute rougher for example, I would have to either add the tool to the end of the list (which makes lookup a pain, I want it between 2 and 3) or I would have to re-number each tool; starting with the last number and adding one, in order to make space for a new tool. Would it be possible to insert a tool between tools and have the numbers below it automatically re-numbered? Having the tools linked to an Excel file would be cool!

I also messed around with the tool libraries to keep things simpler (to me), and created tool libraries for all ball, end, and roughing endmills. However, when I create a new cam style variant, and chose a tool, I can only chose from the full list of "Default-Inches"...also, the diameter and profile aren't automatically set...which defeats the purpose of the libraries.

However, in a PART, if I specify a library, I can choose from tools only within that library for the MOP, which makes sense because of the hierarchy. The diameter and profile still aren't automatically set though.

NOW, in my different libraries, if I start numbering all tools from the number 1, will this cause a problem in the G-code? Say I wanted to use a 3/8 rougher, endmill, and ballnose, in that order. These are all Tool #1 in my separate libraries. Will I get a pause in between the tools? My guess is "no". Just checked, no M6 is generated.

On another note, I'd like to see the double clicking option set for all fields. Like when I double click on Tool Profile, I can change from unspecified, to ball to bull to endmill, etc. Some fields don't have this capability.

Also, CTRL+W doesn't work, can't find the option to show cut width.

I like the new changes vs 097 though, looks promising!
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on January 03, 2011, 15:36:29 pm
Sorry to jump in late on this post, but I seem to be having a similar problem: when I generate my gcode, I get an M3 line without any spindle speed controls. 
...
I can send you a simple .cb file if you want.
Yes please bikegeek, a .cb file would help.

It is possible to get an M3 without an S if the S register has been set further up the file and has not changed,
and your spindle directions have changed between machining operations.

Title: Re: CamBam plus 0.9.8
Post by: 10bulls on January 03, 2011, 16:27:38 pm
Trying to get my head around the tools functions in the new release. Hopefully this makes some sense.

In the "Default-Inches" library, changing a tool's property, index, etc changes the description automatically. It doesn't do it with libraries I created. It's frustrating to have to re-enter my custom description if I am changing something about the tool.

If you click on the 'Default-in' tool library, you should see a property called ToolNameFormat.
This is a macro string that builds the name of the tool from various parameters.
The one for Default-in should read...
{$diameter}" {$flutes} flute {$profile}
If you copy this into your new tool library, tools will be named according to that macro whenever properties change. The automatic name can be overridden by typing into the tool's name field.

If you change the tool name format macro you can also right click the tool library and select 'Rename all tools', which will generate new names for each of the tools in the library based on the new pattern.

You can insert new tools at a given index just by entering in the index of the new tool.  Existing tools from this index onwards will be automatically shuffled up.

Quote
Having the tools linked to an Excel file would be cool!

I agree.  I also appreciate other comments that it is a bit of a pain to maintain tool libraries between a number of different programs (CamBam, Mach3, simulator for example).
The current tool maintenance is very basic at the moment.  The main aim was to get the basic functionality in place in 0.9.8, then develop it further in coming releases.
I think a great idea would be to provide some extra tool maintenance functionality as example CamBam plugins, to provide the opportunity for people to customise these to interface a variety of systems.
More examples, documentation and support of plugins is a high priority for 2011.

Quote
However, when I create a new cam style variant, and chose a tool, I can only chose from the full list of "Default-Inches"...also, the diameter and profile aren't automatically set...which defeats the purpose of the libraries.

Yes, that is not good... I will definitely sort that in an update soon.  It is a little tricky at the moment as the link between the style and the tool library is a little fuzzy.  The style only specifies the tool number, so the actual tool can vary depending on which tool library is selected in the part.

A simple change would be to display the tools in the drop down list from the tool library that is specified in the active part or machining object if no library is set in the part.

Quote
However, in a PART, if I specify a library, I can choose from tools only within that library for the MOP, which makes sense because of the hierarchy. The diameter and profile still aren't automatically set though.

Yes, Jarkman brought up a similar comment recently.  Currently, only machining operations support the new style property values that can inherit from the parent style and display that default, inherited value.
The plan is to extend this to other objects like the Machining -> Part hierarchy as it does make things a lot more obvious and intuitive.
The heirachy still works though.  If you set a tool number in a part, the tool diameter for that tool won't be displayed in the part level (yet), but you should see the resulting tool diameter inherited by the MOPs in that part.  If the part tool diameter is non-zero, this in effect overrides the default tool diameter.

Quote
if I start numbering all tools from the number 1, will this cause a problem in the G-code?

Yes, as you have found this does confuse things.

In an earlier version of 0.9.8 I experimented with using another object 'Tool Palette' as well as 'Tool Library', so you could put tools from the library into a palette then select a palette for the machining or part object rather than a library. 

While perhaps closer to the real world, I felt this just added another level of complexity that wasn't really necessary.

So instead I would treat Tool libraries as dual purpose.  You could put all your tools into a number of logical libraries as it sounds like you are doing, but for machining I would use add another tool library and think of it as your current tool palette.  You can then copy and paste the tools you want from the other libraries into this palette.  In your drawing you would then select a current palette rather than a specific library and all the tools in the palette would have unique indexes.

Quote
On another note, I'd like to see the double clicking option set for all fields. Like when I double click on Tool Profile

OK, I'll look into that.

Quote
Also, CTRL+W doesn't work, can't find the option to show cut width.

Cutwidths and the other view related options got moved to the top object in the drawing tree.
This seemed a more logical place than the machining object.
There is a quicker way to get to it now though, by right clicking the drawing and toggling 'Show cut widths'
from the View context menu.

Quote
I like the new changes vs 097 though, looks promising!

Thanks!  There have been been a lot of changes in this release.  Some features definitely need
improvements but with great feedback like this I am sure they will soon be kicked into shape.
Many thanks for the comments, they are extremely useful and most appreciated.
Title: Re: CamBam plus 0.9.8
Post by: bikegeek on January 04, 2011, 01:54:02 am
Sorry to jump in late on this post, but I seem to be having a similar problem: when I generate my gcode, I get an M3 line without any spindle speed controls. 
...
I can send you a simple .cb file if you want.
Yes please bikegeek, a .cb file would help.

It is possible to get an M3 without an S if the S register has been set further up the file and has not changed,
and your spindle directions have changed between machining operations.
Sorry - it was a misconfiguration on my system, although it may be an installation bug? 

I've got CamBam installed on windows 7, for some reason, it's looking for the "post" folder in the directory I normally save my drawings.  I just noticed the error message "Library path not found: c:\Users\...\Drawings\post" in the message area.  I didn't have a "post" folder, so I found the "post" folder in c:\ProgramData\CamBam plus 0.9.8.  I copied the contents of that folder into the drawings folder and now I get S commands in my .nc files.

So, it sounds like I've got something mis-configured.

Sorry for the false report... I should have paid more attention to the error messages.


Title: Re: CamBam plus 0.9.8
Post by: dh42 on January 04, 2011, 02:59:15 am
Hello,

Andy explains the change of post-pro filepath on this thread ...  ;)

http://www.cambam.co.uk/forum/index.php?topic=1196.msg7515#msg7515 (http://www.cambam.co.uk/forum/index.php?topic=1196.msg7515#msg7515)

++
David
Title: Re: CamBam plus 0.9.8
Post by: rezcar on January 04, 2011, 06:48:48 am
My tool libraries disappeared???


If you click on the 'Default-in' tool library, you should see a property called ToolNameFormat.
This is a macro string that builds the name of the tool from various parameters.
The one for Default-in should read...
{$diameter}" {$flutes} flute {$profile}

Thanks! That gets me further along, I tried to add another variable called {$partcode} or {$notes} in the hopes of getting more info in the description, didn't work. I'd like to be able to add something like rougher, or tapered, or for aluminum. Adding it to the ToolProfile list might make it too long for other users. I guess using the libraries is another option.

Quote
You can insert new tools at a given index just by entering in the index of the new tool.  Existing tools from this index onwards will be automatically shuffled up.
It didn't do it for me, it created another index with the same number, two #4s, etc.
I do get an error message of duplicate tool.

Quote
While perhaps closer to the real world, I felt this just added another level of complexity that wasn't really necessary.
The danger of making a "does it all" program is indeed the complexity! But I think your direction right now is making things easier, such as defining stock materials, and the CAM styles.

Thanks for showing me how to turn on the cut widths ;D
Title: Re: CamBam plus 0.9.8
Post by: brelstad on January 12, 2011, 00:43:23 am
Hi,
I'll be using CamBam for PCB isolation much of the time. Will the next version be able to import the Gerber apertures "oval" and "polyline"?

This would be a great improvement, as most IC pad-layouts has either oval or wide polyline pads as standard.

On some PCB boards, symmetric pads tends to loosen after drilling. Wider pads are much more rigid and they are also a lot easier to solder by hand.


Thanks
Bengt
Title: Re: CamBam plus 0.9.8
Post by: brelstad on January 21, 2011, 17:26:39 pm
There seems to be one bug left in the GDI display mode.

I've got two monitors, in portrait configuration, and use the GDI mode (OpenGL doesn't work in this configuration).
The only problem is that when I hold down the Alt-key and use the mouse to rotate a drawing, the mouse movement is reversed.

Easy fix?
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on January 25, 2011, 10:18:07 am
If I use a Tangent for the LeadInMove it works OK, but if I combine it with a SpiralAngle then the lead-in toolpath 'flips' as shown in the second picture.

Martin.
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on January 25, 2011, 13:50:27 pm
Thanks Martin,

Fixed now in the development version.  Looks like a job for a 'J' release.  I hope I don't run out of letters before we make it to latest stable release!  :-[
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on January 25, 2011, 14:53:03 pm
I have done some investigation into this but I am having problems recreating the problem.

My Nvidia card will happily switch to portrait mode and CamBam with OpenGL works fine.
What graphics card are you using?
Have you tried updating to the latest graphics drivers from the card manufacturer?
There are also a couple of different OpenGL driver implementations available.  I will look into this as maybe trying a different one will help.
My biggest suspicion though would lie with the graphics driver.

I also tried portrait + GDI which also worked as I expected. 
One thing I would say with GDI mode, sometimes rotation can be deceptive and the order lines are drawn can affect how depth is perceived.  For example if you have a rotating wireframe model with no other depth cues, you brain can flip from perceiving it as rotating clockwise to suddenly rotating counter clockwise. A Necker cube is another example of this.
In CamBam's tools - options settings there is a group- 'Mesh Options' and in there a property called BackFaceCulling.  If you set this to False it may help with depth perception when looking at 3D meshes in wire frame mode.

If that is not the problem with GDI you are seeing then I shall go back to being confused and investigate further.
But as far as I can tell it *should* be possible to get this to work with OpenGL also.


There seems to be one bug left in the GDI display mode.

I've got two monitors, in portrait configuration, and use the GDI mode (OpenGL doesn't work in this configuration).
The only problem is that when I hold down the Alt-key and use the mouse to rotate a drawing, the mouse movement is reversed.

Easy fix?
Title: Re: CamBam plus 0.9.8
Post by: brelstad on January 25, 2011, 22:11:11 pm
I loaded the test file referenced by a forum member (Body3D/Corps0.cb). You're right, in GDI mode my eyes was fooled (she did have a nice body...).

As for the OpenGL problem, the image, and mouse movement, is rotated by 90 degrees.
It turns out that Alibre, and a few other graphic software packages has the same problem.
My graphics card on that computer is ancient, Matrox Pharelia 256 PCI, with the latest drivers.
Guess it's time to retire the thing.

I'll buy a new computer soon, until then I'll just use CamBam in GDI mode, problem solved.


Thanks a lot,

Bengt
Title: Re: CamBam plus 0.9.8
Post by: bkamen on February 13, 2011, 17:58:06 pm
Hey all,

 I'm curious if there's a motive behind the uniquely named install dirs for every release of CamBam.

Wouldn't it make more sense in 9.8 and the shared libs in Allusers/Application Data/

to just be named "CamBam Pus" and not "CamBam plus 0.9.8"

I'm just curious - maybe something's been worked out for this already.

Cheers,

 -Ben
Title: Re: CamBam plus 0.9.8
Post by: EAC on February 13, 2011, 21:34:05 pm
Ben,

It done that way so 9.7 and 9.8 can be loaded at the same time.  Some people go back to 9.7 from time to time, and some people are still working in 9.7 til they fully learn 9.8

Don @ EAC
Title: Tab oddity
Post by: mhackney on February 16, 2011, 14:43:18 pm
Hi, I am using the latest 0.9.8 release to make flat disks (.032") in brass that I cut using Mach3 on a Sieg X2 minimill. I use 2 tabs on these disks (about 3" in diameter) to keep them in place. The odd thing is that when I cut the parts, the first tab doesn't get made or it is much smaller than I programmed it to be. the 2nd tab turns out perfect. I have tried several different test parts, used tangential lead in (the first tab gets cut right at the start of the program) and even move the start location away from the first tab. In all cases that "first" tab is not the proper size. I'll post the code when I get home tonight but wanted to check if this is a known problem that others have experienced.

cheers,
Michael
Title: Re: CamBam plus 0.9.8
Post by: pixelmaker on February 16, 2011, 15:54:22 pm
hello mhackney

no, I have no problems with the tabs.
Perhaps you can upload a .cb file that we can see it?

Title: Re: CamBam plus 0.9.8
Post by: c.sitas on February 16, 2011, 15:59:21 pm
Hello  mhachney;   I had this once and it turned out to be my set up .  Everything was not "dead nuts on". I reset my Z axis to as near perfect as I could. The problem went away. This is just a thought. c.sitas
Title: Re: CamBam plus 0.9.8
Post by: dh42 on February 16, 2011, 16:48:38 pm
Hello,

I had this problem with slim parts, but it is not related to cambam, my part is pulled upward by the spiral of the mill and it cuts the tab in passing.  ::)

++
David
Title: Re: CamBam plus 0.9.8
Post by: blowlamp on March 16, 2011, 09:04:39 am
I'm having a few problems machining a mould with the attached file.
The picture shows that CamBam is causing a small overcut at the pointy end if I use any postprocessor other than Default.
The opposite end also cuts in an odd way, but might be to do with the step on the model of the part.



Martin.
Title: Re: CamBam plus 0.9.8
Post by: dh42 on March 16, 2011, 13:45:45 pm
Hello Martin,

I try your file and get same problem with CV, and CNc simulator say an error on the file !!

I look the toolpath with step by step in CV with trace "on", and toolpath seems to be right  ???  ... you have this problem on the real part ? or just on simulation ?  maybe a CV bug ?

Edit: it's not possible to obtain this square angle with the mill !!

++
David
Title: Re: CamBam plus 0.9.8
Post by: 10bulls on March 16, 2011, 21:33:23 pm
I found the lines where CV was having that glitch, created a small gcode excerpt and loaded that into Mach3.
This loaded OK and the toolpath looked good.

There was a rather large diameter arc there, so hopefully this is just a precision glitch in CV.

I just reduced the maximum arc radius setting in my Mach3-CV post processor from 100000 to 10000 and reran the file.  This worked OK in CV with no snaggles.

I think the opposite end is due to the stepover setting.  You could try reducing the stepover or adding a roughing clearance to prevent it overcutting that bit.

Good luck!

Title: Re: CamBam plus 0.9.8
Post by: blowlamp on March 17, 2011, 09:12:59 am
Thanks for looking at that for me, Andy.

Changing the MaximumArcRadius fixed the overcut problem at the rounded end, but my fiddling with the StepOver setting hasn't sorted out the problem at the other end.

Due to how I've got to make this part, it won't matter because I've got to cut this longer than really needed and then trim it back anyway.

Here's another file that's been giving me some jip, because it's struggling with the LeadIn moves in two ways.

The first problem is shown in the picture as an overcut on the corner of the part (which I think is related to ToolDiameter and the MaxCrossoverDistance).

The second problem shows as an error message when I set AdjustCutWidth to True under the SideProfile option.

Thanks again.

Martin.

Title: Re: CamBam plus 0.9.8
Post by: 10bulls on March 17, 2011, 18:25:34 pm
It is indeed the MaxCrossoverDistance to blame.

CamBam is just following orders! ( ::) ) in that the lead in start point is ~4mm away from each layer's toolpath end point.  The tool is quite large relative to the size of the part so a 0.7 MaxCrossoverDistance x 10mm tool diameter is 7mm.

That means the post processor is 'allowed' to do a feed move when the start of the next toolpath is within that distance from the end of the previous toolpath.

Reducing the MaxCrossoverDistance to 0.4 (4mm with a 10mm cutter) makes the problem go away as the distance back to the lead in start is larger than the max crossover distance so a plunge via the clearance plane is forced.

I think the naughtiest thing is that CamBam does not display the crossover feed moves (these are currently insert by the post processor code, after the toolpaths have been generated).  Displaying these moves is on the TODO list.  As well as giving a better representation of the actual toolpath this will also help improve the cutting time estimates.