Author Topic: Rest machining - for me, the "only" missing feature in CamBam!  (Read 12885 times)

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1356
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #45 on: February 12, 2020, 00:25:12 am »
HI Sibianul

Those lines are malformed because the underlying geometry has issues, this causes what you are seeing.
There is a companion plugin here that will clean and repair the geometry.

I had to make this plugin because if you are using a file made by another cad program especially files
from the internet or have used CB functions to cut up and join the geometry (break at intersections)
is a common villain then you should run the file cleaner over the geometry to make sure that it has no
duplicate entries in the line.

It can be this issue here:
http://www.cambam.co.uk/forum/index.php?topic=4945.msg62407#msg62407

A lot of common problems that you might experience at the start of using the plugin are
explained in these threads:

http://www.cambam.co.uk/forum/index.php?topic=4945.0

This thread is where I first started writing the plugin and has some useful info as well.
http://www.cambam.co.uk/forum/index.php?topic=4665.0

The file cleaner:
http://www.cambam.co.uk/forum/index.php?topic=4924.0

For a plugin that started out with a simple premise, it quickly escalated into a
nightmare as the underlying complexity of doing it became apparent.

You can use the CC in a few different modes, for example if you don't generate
the mops then you should get closed polylines, if you don’t then there is something wrong with the geometry.
If you generate the lines with the mops checked then you should get open polylines.

Also if you want to keep a layer untouched between generating new lines then rename the layer.
There are times when you may need\want to do this.

If you can post that small segment of your file (the top left hand corner) I will look at it and explain
the issues found and provide a solution.

Dave

Offline sibianul

  • Wookie
  • ****
  • Posts: 278
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #46 on: February 12, 2020, 14:47:33 pm »
Those lines are malformed because the underlying geometry has issues, this causes what you are seeing.
There is a companion plugin here that will clean and repair the geometry.
Just a short reply Dave as I'm quite busy :(, the lines are NOT malformed, are exactly how they should be, maybe I wasn't clear, it's just I had to draw the arcs to join OPEN lines toghether, because only when the lines are closed, Cambam could detect the collision when doing the slope profiles.

PS. I milled the part and it came out perfect :) I'm just posting the file to make things clear, maybe I wasn't clear enough in my previous message. I exploded the left corner so you see how the slope profile is milled if the lines are not closed. For simple models like this I will definitely use your plugin more often, even If I will have to manually join the lines together, it's more riskier on complex models, where there are many small unmilled corners .. but in time I will let you know how it goes. After this part that  milled yesterday, I'm quite happy, the plugin is very useful :)
« Last Edit: February 12, 2020, 19:43:35 pm by sibianul »

Offline dave benson

  • CNC Jedi
  • *****
  • Posts: 1356
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #47 on: February 13, 2020, 01:08:24 am »
HI Sibianul

Malformed was probably a wrong term as you can not see the problems with the geometry on the screen
even though there is.

The insidious thing here is, within reason the cam part of CB will ignore those errors and
generate you a good mop most of the time.

For example say that you generated the a mop with a 3mm cutter and a stepover of 0.7
and generate the tool paths and run the job and everything works out OK, and then a
few months later you go to do the job again but have broken your 3 mm cutter and use
a 3.175 mm cutter and change the stepover to suit and all of a sudden the tool paths
wont be correct any more leaving you wondering what happened as it worked before.

The screen shot is of another Plugin (I have all of them installed)  also complaining
about some of the geometry I could go on and explain exactly what happened here
but it would take a long time, suffice to say some of the lines need to be cleaned
either with the built in functions of CB or the file cleaner.

I'm going to a little busy myself today as my laser has come and I have made the spindle mount and fitted it
to the mill and hope to make some 2.7 mm neoprene gaskets without burning the place down.

Dave

Offline tsikows

  • Ewok
  • *
  • Posts: 14
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #48 on: May 01, 2020, 15:02:15 pm »
Has anything come of the Rest Machining feature request? I realize this is a dead thread but after reading through it im no closer to understanding a workaround than i was before.

Offline sibianul

  • Wookie
  • ****
  • Posts: 278
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #49 on: May 01, 2020, 15:21:24 pm »
@tsikows, have you tried the COLLISION DETECTOR plugin?

It does work but you need to manually fine tune the generated lines.

Unfortunately I think I was one of very few people that needed this function, when working with Fusion360 I use this function on all my steel dies, without it the time needed to mill the steel parts would be much higher, as I mention when I opened the thread, for me this is quite important and I say it again, I would pay an UPGRADE FEE, let's say $50 - it would be ok for me, if this function would be available, and I'm sure others would agree to pay a fee for this upgrade.


Offline Bob La Londe

  • CNC Jedi
  • *****
  • Posts: 3988
  • ^ 8.5 pounds on my own hand poured bait.
    • View Profile
    • CNC Molds N Stuff
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #50 on: May 04, 2020, 21:13:05 pm »
First thing to point out is this thread has been read over TEN THOUSAND TIMES. 

Rest machining is a big deal for complex work.  Its a huge time saver over doing something like a finish pass of an entire work piece with a tiny mill.  Its astronomical.  Logarithmic. Gi-hugic. 

Often I can do a mediocre work around by creating secondary geometry and using the secondary geometry to do pseudo rest/finish machining, but its a huge kludge in the back side.  When I get into complex 3D molds (or dies) I sometimes don't even realize things have not been finished in fine details until the mold is tested.  They don't get tested in place on the mill.  Putting them back on the mill (or other machine) later and picking up their location again is another huge time suck, and I never trust it to be perfect. 

When I say I would love to see rest machining I mean 3D rest, but I can see some value in 2D work as well. 
Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com

Offline tsikows

  • Ewok
  • *
  • Posts: 14
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #51 on: May 07, 2020, 00:33:41 am »
sibianul I did downlaod the "collision detector" as well as the "uncut areas" plugins. I was able to play with both and found them to be reasonable options only if you have spare time on your hands to dink with it, but for me neither would be a suitable workaround as there is a much simpler solution called Carbide create. It is able to build me a toolpath with two cutter sizes and automatically calculates where the big one missed and creates the path for the smaller tool aswell. Saddest part about Carbide Create is its totally free.

Offline onekk

  • CNC Jedi
  • *****
  • Posts: 512
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #52 on: May 07, 2020, 08:27:51 am »
Yes but Carbide Create is only a 2D cam and CamBam has some 3D functions, plus Cambam is very expandable with plugin.

Plus it work even on Linux, in fact a part from FreeCAD that have a Path WorkBench, CamBam is at my knowledge the "only viable solution" to do a decent CAM with Linux, it is not free but quite cheap.

Regards

Carlo D.
Carlo D. (onekk)

eShapeoko #343 750x1000 mm + GRBL + bCNC + CamBam

Offline sibianul

  • Wookie
  • ****
  • Posts: 278
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #53 on: November 14, 2020, 17:03:12 pm »
...but for me neither would be a suitable workaround as there is a much simpler solution called Carbide create. It is able to build me a toolpath with two cutter sizes and automatically calculates where the big one missed and creates the path for the smaller tool aswell. Saddest part about Carbide Create is its totally free.

Hy, I just tried Carbide Create , for simple and big parts probably Carbide Create is great, but for complex and small parts, Carbide Create is just a joke :)

I played with it about 15 minutes, and found 2 serious issues (maybe there are some workarounds, but I haven't noticed any)

1. When defining tools there is no option for TOOL TIP DIAMETER



2. It seems the MAXIMUM RESOLUTION of Carbide Create is not high enough for small details, In my example I have some SMALL letters  (the smallest in this model is 1.3 x 1.5mm). If you check the toolpaths and also the imported DXF file, there are many straight lines instead of arcs, the toolpaths lines don't follow the contour of the letter.

So, Carbide Create is not usable for small parts.


---------------------------------------------------------------------------------------

Back, to CamBam now :)  yesterday and today I tried today to optimize even more my workflow, my main problem is that I'm losing time milling air, on the exterior regions of the models, on areas where I already milled using a flat end mill. I'm losing time because I use a very small 0.2mm tip  V-cutter, the feed is around 100mmpm and DOC is 0.1mm sometimes the Target depth goes to -1

While the REST MACHINING option is still missing, I tried 3 new strategies, hoping I can mill the parts faster.

1. I usually use the 2mm Flat Endmill to mill around letters, with an additional 0.2mm ROUGHING CLEARANCE , than I start milling with V-cutters, 1mm tip, 0.5mm tip and 0.2mm tip size, the last two operations beeing the most time consuming, as the feed is quite slow, around 100mmpm and a 0.1mm DOC.
Yesterday I had a new ideea to create an offset contour around the entire word to limit the AIR MILLING TIME, and it worked great, instead of 35 minutes now it mills the same thing in 27 minute, but it still mills AIR, as you can see in the photo attached, it mills on the interior of the new contour created and also on the exterior of the letters, until the toolpaths meet. It would be perfect if I could just use the same Slope Profile MOP but limit the area to the selected contour, like the BOUNDARY option of 3D profile MOP , this way it will mill on tight space, and on exterior sides where the material is already removed by flat endmill, will only make about 2 passes.



2. Then I wanted to try to mill using 3D Profile MOP because I knew this operation has the BOUNDARY feature that can help me save some time . If this option was available for normal 2D Profile MOP it would be a good alternative to rest machining, but still would need time to manually create shapes to avoid milling air, but less time than the COLISION DETECTOR plugin, which for detailed models  is very time consuming.
The problem with 3D Profile MOP is that it doesn't care about the TOOL PROFILE, when I used the same 30 degree V-Cutter, the toolpaths generated should look very similar with the above attached, Slope Profiles MOP's, but instead the toolpaths is exactly like it is would be when milling with flat endmill.

Probably an possible solution to this, is to model the solid surface, with the angled walls, instead the straight vertical walls, BUT I DON'T KNOW HOW TO DO IT IN CAMBAM, I can do it in Fusion360, but Fusion360 has his own issues with those imported DXF files.

Fun fact: Today I was laughing with my colleague because on one stamp I was working, it took a little bit more than expected for Cambam to generate the toolpaths, about 20 seconds , and while I was waiting my colleague seen me I was smiling/laughing alone, he asked me : What's Up ? I responded: I just imagined how Fusion360 would crash when trying to import this same model, that has a few thousands segments  ;D In cambam I just used the Arc fit option, and the time reduced to less than 5 seconds. In Fusion360, after many posts on their forum, the most common solution is : "You should try to redraw the entire sketch, in fusion, and not import that garbage dxf...."



3. Vcarve MOP. I tried this in the past and I noticed that on some small features, the model was overcut, I tried again now and the toolpaths looks ok but there still is something missing:

  • The DEPTH INCREMENT option is missing, and I don't think that the 0.2mm V-cutter will last to long when plunging in the Brass material, if anyone has any experience, please share it. I would try again, using the spindle RPM close to 20k , maybe this way it will work better.

Monday if the machine will be free of jobs, will try a sample with V-engrave plugin, to see if it will mill ok. I have some doubts, but will let you know after milling a test part.

So, long story short:
1. The 2D Profile MOP with the SIDE PROFILE option set to SLOPE, is great, but it's missing the BOUNDARY option!
2. 3D Profile MOP has the BOUNDARY option, but it doesn't care about the TOOL PROFILE I set, and it will overcut the model when milling with a V-Cutter.
3. V-Engrave it also looks good, but it's missing the DEPTH INCREMENT option, and option that all other MOP's have.
« Last Edit: November 14, 2020, 17:20:01 pm by sibianul »

Offline sibianul

  • Wookie
  • ****
  • Posts: 278
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #54 on: November 14, 2020, 17:26:00 pm »
I was limited to 5 attachments in my previous post, so here is the model I was playing above

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4565
    • View Profile
Re: Rest machining - for me, the "only" missing feature in CamBam!
« Reply #55 on: November 14, 2020, 19:26:21 pm »
With the v-engrave plugin it's possible to create one MOP with all your settings, then copy and paste it to create more of them. In each one set the "Max Depth" to a little more each time until you reach full depth.


Edit: But I see you already used that method.
« Last Edit: November 14, 2020, 19:37:52 pm by EddyCurrent »
Made in England