First Post, First Project, & Some Questions

[lloydsp]

Kelly,

"Boring holes vs Pockets: When boring holes much larger than the bit diameter, is there any advantage/disadvantage to the drilling with either spiral or canned method? or alternately, just cutting them as a pocket? I did the throttle bores as spiral drilled and as pockets and the tool paths seem to display very similarly."
--
I tend to pocket such holes.
--
"Roughing: I see roughing displayed in the various machine ops. Is a roughing and finish cut available in all machine ops or just 3D? For example, could I make successive cuts of increasing depth leaving say .030" of stock on a profile or pocket and then make a full depth finish cut?"
--
Roughing and finishing are available in 2.5D ops, as well.
--
"Tool Path Visibility: The documentation says you can select "Tool Path Visibility" to display either selected items or all and also that this was moved to the first item in the drawing tree for 1.0 but I can't seem to find where to toggle between selected and all objects/MOPs. Where is it?"
--
I don't know about that one.  I've not challenged it, because I use a simulator to view what the work will be like.
--
"Order of machining operations: When the gcode file is generated, will the MOPs be executed in the order the appear in the machining tree?"
--
Yes!
--
"Bitmap vs Vector file. I was reading through importing a Bitmap or image file. There are several logos and images I would like to scale and reuse on future projects. I see I can download them in about any image file or vector file. What's the vector file? It's has an .svg file extension, correct? Does it just break the link to the bitmap and imbed in the CamBam file? And which would be best to download and save for scaling and repeated use of an object generated from an image? It appears the Script function could also be a candidate for same but not sure I understand the advantage/disadvantage over the former."
--
I don't use such.  I design my parts IN CamBam.  Sorry I cannot help more.
--

Lloyd

[EddyCurrent]

Tool Path Visibility

Select  File->New, you will see right at the top "Untitled", click on that and the options will pop up.

SVG files

These are not supported by CamBam's core code, the option was added by way of user written plugins. Vector files are generally referred to as "scalable" because they can be scaled without loss of information unlike a jpg file for example.
 I use them for my laser which recognises Red, Blue and Black for different operations. The most popular software for creating vector files is Inkscape; https://inkscape.org/ and it's open source and free to use.
In the case of CamBam SVG files might be regarded as an alternative to DXF files but my recommendation would be to use DXF files rather than SVG.
Only Bitmaps can be used to create a surface for 3D work.

[dh42]

Hello

1) I prefer to use the spiral milling on holes that are almost the same size than the tool because with pocket, sometime CB won't generate toolpath if the tool size is close to the hole size.

2) Rouhing property exist on all MOP but they have no effect, except for 3D MOP and Lathe MOP

on the doc

Roughing / Finishing    

Currently only supported by 3D Profile and Lathe machining operations.

3) see picture .. and also have a look on the "View/toolpath view filter", it is a very useful tool
http://www.cambam.info/doc/dw/1.0.0/view-menu.html#ToolpathFilter

4) yes

5) it is better to use vector files (like DXF or SVG) than bitmap. In all case, CB needs vector drawing, so if you use a bitmap the outlines must be extracted from the bitmap ... and this don't give always nice results (lines have stairs because pixels)

You can use the bitmap object to extract the outlines of a bitmap

http://www.cambam.info/doc/dw/1.0.0/cad/bitmap.html

++
David

[Garyhlucas]

Kelly,
You likely can’t use canned cycle drilling in GRBL unless it recognizes G80,G81, codes which are called modal commands. Call once and it repeats the drilling operation after every rapid move.  Spiral drilling works up to twice the diameter of the end mill, then it will leave the center uncut. I often drill twice with a second circle to take out the middle first. I use pockets only for very large round holes with a small tool to avoid a tool change.

Roughing is best done using a rough MOP with appropriate clearances. Lie about the tool size, making it bigger works.

When I first came to CamBam I had lots of experience with 2D and 3d cad so I really didn’t care that it had almost no drawing tools. Lots of people asked for drawing tools and they got added. I draw simple stuff in CB but for something like your manifolds I would definitely use a dedicated cad program for design as all of them have better tools for drawing than CB. CB can do it but it isn’t always easy or quick.  If you haven’t done so already you need to download all the plugins that clever people here have written as many of them are hugely useful.

[dave benson]

Hi Kelly

I wrote this plugin which gives any controller including the GRBL folks access to all of the Drilling canned
cycles in the Gcode standard and any drilling custom canned cycle's that you may dream up, as well as full rigid tapping
with machine and hand taps, also the canned cycles show up in the Camotics simulator so that you can get a
good idea of what the machined surface actually
looks like.

https://cambamcnc.com/forum/index.php?topic=8346.msg66325#msg66325

As your just starting out with GRBL you should consider this plugin below as it'll save
you a lot of grey hairs, it's tightly integrated with CB and works well and is really one of those
must have plugins if you have an GRBL powered machine.

https://cambamcnc.com/forum/index.php?topic=6482.0

Happy cnc'ing.

Dave

[Tool-n-Around]

Thanks for all the reply’s fellas. They’re very helpful.

Boring holes vs Pockets

........1) I prefer to use the spiral milling on holes that are almost the same size than the tool because with pocket, sometime CB won't generate toolpath if the tool size is close to the hole size.

That’s good to know. On this part I was drilling 5/16” holes with a ¼” cutter but the other slight benefit of a pocket seems to be I can see the hole size on the drawing when it’s a circle/polyline vs just a point for drill location.

You likely can’t use canned cycle drilling in GRBL unless it recognizes G80,G81, codes which are called modal commands. Call once and it repeats the drilling operation after every rapid move.

Also good to know.

Spiral drilling works up to twice the diameter of the end mill, then it will leave the center uncut. I often drill twice with a second circle to take out the middle first. I use pockets only for very large round holes with a small tool to avoid a tool change.

I figured it’s a matter of tool change versus run time. When I pocketed the 2.25” holes with a ¼” cutter, I called for .9 stepover……but haven’t made chips yet.

Roughing

2) Roughing property exist on all MOP but they have no effect, except for 3D MOP and Lathe MOP......Roughing / Finishing Currently only supported by 3D Profile and Lathe machining operations.

Noted, thank you.

Roughing is best done using a rough MOP with appropriate clearances. Lie about the tool size, making it bigger works.

Oooh…that’s a good one. I see some metric bits in my future for making undersize cuts.

Tool Path Visibility:

3) see picture .. and also have a look on the "View/toolpath view filter", it is a very useful tool http://www.cambam.info/doc/dw/1.0.0/view-menu.html#ToolpathFilter

…..Select  File->New, you will see right at the top "Untitled", click on that and the options will pop up.

Ahhh, got it now. I wasn’t looking in the top level drawing object. Thank you!

Bitmap vs Vector file

You can use the bitmap object to extract the outlines of a bitmap.

5) it is better to use vector files (like DXF or SVG) than bitmap. In all case, CB needs vector drawing, so if you use a bitmap the outlines must be extracted from the bitmap ... and this don't give always nice results (lines have stairs because pixels)……You can use the bitmap object to extract the outlines of a bitmap[http://www.cambam.info/doc/dw/1.0.0/cad/bitmap.html

….These are not supported by CamBam's core code, the option was added by way of user written plugins. Vector files are generally referred to as "scalable" because they can be scaled without loss of information unlike a jpg file for example……….In the case of CamBam SVG files might be regarded as an alternative to DXF files but my recommendation would be to use DXF files rather than SVG. Only Bitmaps can be used to create a surface for 3D work.

I’m going to have to experiment with this. There are things like logos and words in proprietary text fonts that I will reuse on multiple projects, but they will likely need to be different sizes thus the interest in scaling.

Thanks again gents.

Best,
Kelly

[Tool-n-Around]

......I draw simple stuff in CB but for something like your manifolds I would definitely use a dedicated cad program for design as all of them have better tools for drawing than CB. CB can do it but it isn’t always easy or quick.

I’ve gathered this to be the case. The interior runner geometry isn’t optimal. I’d like to drive a 3D spline that starts as a round cornered rectangle and then blends and finishes to 2.25” circular cross section. Then instead of all the pieces in those runners, it could be a top and bottom for all 8 runners that gets glued together. I’ve started using Fusion but little steeper learning curve there. I suppose there is a chance that after being modeled it could be cut in CB but fusion also has CAM. Just a matter of how well GRBL will do in the 3D ball nose step over cutting. 90% (at least now) of what I do for lost foam pattern work can be drawn and cut with CB……

If you haven’t done so already you need to download all the plugins that clever people here have written as many of them are hugely useful.

I’ll have to do that Gary, thank you. Case in point below...

…..I wrote this plugin which gives any controller including the GRBL folks access to all of the Drilling canned cycles in the Gcode standard and any drilling custom canned cycle's that you may dream up, as well as full rigid tapping with machine and hand taps, also the canned cycles show up in the Camotics simulator so that you can get a good idea of what the machined surface actually looks like.

Thank you. I'll download it!

….As your just starting out with GRBL you should consider this plugin below as it'll save you a lot of grey hairs, it's tightly integrated with CB and works well and is really one of those must have plugins if you have an GRBL powered machine.

Thanks much Dave. I bought a MillRight MegaV CNC router and I was probably more focused on the hardware than firmware and software to drive. It should have probably been the other way around. We’ll see how far I can get with it and GRBL. In the near term, it will probably serve its purpose but I may grow weary if/when my CAD skills develop and I attempt more complex 3D surface and machining, but for the time, I like CamBam and can see the benefit of having it on hand.

I've drawn up and generated a couple somewhat more complicated files for this project that will require tool changes and two sided machining. I'll make a separate post on those.

Best,
Kelly

[dh42]

Hello

the other slight benefit of a pocket seems to be I can see the hole size on the drawing when it’s a circle/polyline vs just a point for drill location.

You can also use circle for drilling, in the drill MOP, set "Hole diameter" to auto so the MOP take the hole diameter from the circles. The advantage is that you can cut holes of different diameters with the same MOP.

To set the "Hole diameter" to auto, right click on the small "arrow" icon at the left side of the property to get the context menu.

an example with a property of the V-engrave MOP
https://cambamcnc.com/forum/index.php?topic=3513.msg72183#msg72183

++
David

[Tool-n-Around]

......You can also use circle for drilling, in the drill MOP, set "Hole diameter" to auto so the MOP take the hole diameter from the circles. The advantage is that you can cut holes of different diameters with the same MOP. To set the "Hole diameter" to auto, right click on the small "arrow" icon at the left side of the property to get the context menu.

That's useful. I've been converting circles to poly lines but you loose the center coordinates and diameter which is suboptimal when drawing and editing.

Thanks.

Best,
Kelly

[Tool-n-Around]

Couple more questions:

• I’ve made some minor edits/refinements, generated the corresponding gcode file, and ran a simulation in CAMotics. All looked good but although the machining operations/(parts) were performed in the order each folder/part appeared with the Machine tree, the machining operations did not execute in the order they appeared within each folder/part, and were often split and/or blended. Is this something specific to CAMotics or is it related to the Cambam tool path generation, and should I expect same when the file is executed on the machine?
• Is it necessary to set the stock dimensions and offset in each part in the machining tree when it is already set at the top level of the tree?
• How will the holding tab be treated if it overlaps another machining operation in a different part of the machining tree other than part where the holding tab created? Will the cut in the other MOP execute as created or will it recognize the tab and skip that stock? I could not tell in the simulation or tool path view.

Updated gcode file attached.

If I can get my machine sorted, I’ll be ready to cut soon.

Best,
Kelly

[dh42]

Hello

I've been converting circles to poly lines

Ah yes, it's a good idea to avoid converting circles to polylines, but even with a circle converted to a polyline CB can use the Auto setting to get the diameter.

Currently, there is no way to go back after a circle has been converted to a polyline, but you can retrieve the center with draw/points/center(extended)

If you want to change the diameter, you can "resize" the polyline, but the resize function use the drawing center as transformation center so the location is also changed. Eddy's "In place resize" plugin can be used if only one hole need to be resized.

http://www.atelier-des-fougeres.fr/Cambam/Aide/Plugins/In%20Place%20Resize.html

If you have more than one polyline circle to resize (to the same size), you can use the following method:

- select all circle polylines that must be resized to a new diameter
- use Edit/Explode to convert all polylines to Arcs
- You end up with all arcs selected
- change the radius value for all arc in one shot
- with all arcs still selected, type CTRL J (join) on the keybard to redo polylines
- If the source polyline was linked to a MOP, you have to redo the link to the MOP


++
David

[Garyhlucas]

Kelly,
If optimization is on in a MOP then CB will try to do the cuts in the shortest amount of travel. Turn it off and objects will be cut in the order listed in the MOP.

CamBam writes all the code relative to the origin X0,Y0,Z0. So you have to tell the machine where that is on your material.  Typically the edges of your stock. You might draw the stock size in CB then locate your part on that. Then Select All and move everything so a corner of the stock is at X0,Y0.  On your machine you then pick up the stock edges and set them to zero.

A trick I use that will work for you so you don’t need to switch tools to an edge finder.  I move the tool near the edge of the stock and use a round pin between the tool and the stock. I jog closer than the pin diameter then hold the pin in the gap and jog away until the pin drops.  You are then the pin diameter + tool radius away and you enter that value as your location rather than zero.  I use a pin instead of a shim because jog amounts can be 0.100” and an oops breaks the tool or material. I use a 3/8” pin for setting X,Y, and Z to avoid crashes.

[dh42]

Hello

1) need .cb file to see ... CB execute the MOPs in the order they appears in the tree.

2) no, you can set it in the machining folder only, and it will be used for all CAMparts ; this plugin is very helpful for that
http://www.atelier-des-fougeres.fr/Cambam/Aide/Plugins/MakePartStock.html

3) There is no specific treatment between 2 mops, so you have to place the tabs manually so they overlaps to avoid unwanted cut on others tabs (pic4) .. if the shapes to cut are in the same mop, the tabs are taken in account for the neighbor toolpaths. Pic3 show the results with one mop for 2 shapes or one mop per shapes.

If needed, the length of the tabs can be changed in the Machining folder with Inner Tabs Scale and Outer Tabs Scale properties (tabs lenght is relative to tool diameter)

++
David

[dh42]

If optimization is on in a MOP then CB will try to do the cuts in the shortest amount of travel. Turn it off and objects will be cut in the order listed in the MOP.

Yes, but I thought Kelly talk about the order the mops are cut into a CAMpart, not the order the shapes are cut into a mop ... not sure .. 

The only thing that can change the order the mops are cut into a CAMpart is the use of nesting, in this case if there is more than one tool used, the order can change to optimize toolchange. (GCode Order property)

http://www.cambam.info/doc/dw/1.0.0/cam/nesting.html#output-order-of-machining-operations

++
David

[Tool-n-Around]

......Ah yes, it's a good idea to avoid converting circles to polylines, but even with a circle converted to a polyline CB can use the Auto setting to get the diameter.....Currently, there is no way to go back after a circle has been converted to a polyline, but you can retrieve the center with draw/points/center(extended)

I'll post the other things I've been working on, and it may be a matter of how I'm creating/drawing the parts in CamBam, but I have intersections of lines, rectangles, arcs, and circles used to create part geometry, then break at intersections to eliminate the unwanted bits and join it all back up into a single polyline, but I often can’t succeed if they aren't all polylines. So I just assign a point list for circle and arc center locations and snap to those to reconstruct the circle or arc if needed, but I have certainly made note of the other methods you mentioned. Thank you.
The rest of the replies are noted and understood.

Yes, but I thought Kelly talk about the order the mops are cut into a CAMpart, not the order the shapes are cut into a mop ... not sure .. 

Yes, but I was probably mixing or misusing terminology. The parts under the machine tree to execute in the order they appear but the MOPs within them do not…….but as Gary mentions below…

If optimization is on in a MOP then CB will try to do the cuts in the shortest amount of travel. Turn it off and objects will be cut in the order listed in the MOP.

Voila! That did it. Thank you.

CamBam writes all the code relative to the origin X0,Y0,Z0. So you have to tell the machine where that is on your material.  Typically the edges of your stock. You might draw the stock size in CB then locate your part on that. Then Select All and move everything so a corner of the stock is at X0,Y0.  On your machine you then pick up the stock edges and set them to zero.

So this is the first of five parts I have designed. It is centered on 10x21 stock. The others on 24x12 stock. In all cases I applied offsets from the XY origin of the parts that center the part on the stock and the new offset origin to the lower left corner when viewing XY Plane. So standing in front of my cnc router, if the machine origin is the front left corner with +X to the right and +Y away, I simply place the corner of the new offset XY origin at the machine origin….correct? All  the features of my parts are well within a cutter diameter of the edge of the stock so I figure how precisely it is placed is not of much concern. I have incorporated other registration features for 2-sided machining. I’ll post up those other files for comment. I’m working through some electrical gremlins on my router but think I’m almost there.

1) need .cb file to see ... CB execute the MOPs in the order they appears in the tree.

Sorry, cb file now attached.

Best,
Kelly