CAMBAM - 10Bulls crazy CAD/CAM software project

[santiniuk]

Considering the small timescale of the development so far it's hardly surprising a few issues are cropping up. The great thing now is that this thread is starting to get the attention it deserves and I'm sure it won't be long before CAMBAM develops into an extremely useful piece of software. (As has NCPlot).

Keep coding Andy but remember the rules. 2 food and toilet breaks per a day only

[CLaNZeR]

This is excellent 10-Bulls and running version 0.6 today, it knew there was a newer version and took me to the site for download, so that bit also works well!

I had one thing that killed Kcam when importing the Gcode and this was the comments:

; This file was created automatically using CAMBAM
; http://www.brusselsprout.org/CAMBAM
; 21/12/2005 10:04:33


If I edit the file and changed them to the below, it worked fine and Kcam showed the first part of the Shark that I load from your samples.

[ This file was created automatically using CAMBAM]
[ http://www.brusselsprout.org/CAMBAM]
[ 21/12/2005 11:04:33]

So all looks fine in Kcam, so next I loaded it into CNCSimulator from Microtech and got G03 Illegal endpoint from this line
G03 F200 X0.50803 Y10.1026 I0.38347 J9.93313

But as I said looks fine in Kcam, so do not know if this is CNCSimulator.

Excellent bit of software though.

One other thing should the attached screenshot be correct if I wanted to produce a cuts of 0.2mm using material thickness of 1.2?
As I expected the Gcode to show the toolpath being repeated with 0.2mm increments till it reached Z-1.2 but it did it in one 1 pass at Z0

G21
G90
G00 Z1.5
M03
G00 X0.59337 Y9.91972
G01 F50 Z0
G03 F200 X0.50803 Y10.1026 I0.38347 J9.93313
G01 X0.48262 Y10.12058
G02 X0.48705 Y10.13428 I0.49263 J10.12491
G03 X0.51785 Y10.15405 I0.46403 J10.20404
G03 X0.57828 Y10.2255 I-0.07302 J10.71503
G02 X0.64831 Y10.25138 I0.64341 J10.15697
G03 X0.74303 Y10.26034 I0.67595 J10.46442
G03 X0.94669 Y10.37732 I0.64947 J10.65899
G02 X1.06447 Y10.30286 I0.97119 J10.28569
G02 X1.1411 Y10.10459 I0.6292 J10.02068
G02 X1.25189 Y9.6846 I-30.8081 J1.45243
G02 X1.31888 Y9.38388 I-2.65088 J8.6574
G02 X1.40103 Y8.60189 I-2.77101 J8.5589
G02 X1.36678 Y7.83523 I-5.09761 J8.5081
G02 X1.14613 Y6.68961 I-5.83667 J8.62863
G02 X0.84155 Y5.84666 I-4.65084 J8.30769
G02 X0.68909 Y5.54607 I0.16344 J6.00164
G02 X0.55646 Y5.56628 I0.62717 J5.58503
G03 X0.58664 Y6.28593 I-4.24361 J6.12804
G03 X0.48946 Y6.83005 I-2.41773 J6.03004
G03 X0.36295 Y7.25881 I-8.87923 J4.29885
G02 X0.2768 Y7.62886 I3.75177 J8.24275
G02 X0.23255 Y8.07632 I5.49133 J8.37051
G02 X0.22105 Y8.53043 I12.62124 J8.61736
G02 X0.23739 Y8.88722 I3.60633 J8.55416
G03 X0.25053 Y9.21884 I-2.29491 J9.15364
G02 X0.25736 Y9.29096 I2.04206 J9.08548
G02 X0.29824 Y9.34047 I0.3511 J9.2552
G02 X0.46085 Y9.40263 I0.50076 J9.05443
G01 X0.49268 Y9.41293
G03 X0.51607 Y9.43587 I0.46096 J9.46866
G01 X0.53249 Y9.48252
G01 X0.55413 Y9.59593
G03 X0.59337 Y9.91972 I-1.74928 J10.03932
G00 Z1.5
M05
M02

Best Regards

Sean.

[10bulls]

Originally Posted by CLaNZeR ...I had one thing that killed Kcam when importing the Gcode and this was the comments:

Yes, round brackets for comments also seem more universal... Custom post-processor code should sort this sort of thing.

So all looks fine in Kcam, so next I loaded it into CNCSimulator from Microtech and got G03 Illegal endpoint from this line G03 F200 X0.50803 Y10.1026 I0.38347 J9.93313

I'm pretty sure this is the absolute/incremental issue thing (see above post).

One other thing should the attached screenshot be correct if I wanted to produce a cuts of 0.2mm using material thickness of 1.2? As I expected the Gcode to show the toolpath being repeated with 0.2mm increments till it reached Z-1.2 but it did it in one 1 pass at Z0

Sorry, the terminology and layout is pretty confusing at the moment...

The ZFinal parameter is the depth of the final cut (ie the finishing pass), so in your example the last cut depth is 1.2mm which is the same as the total depth. Set ZFinal = 0 and you should be right.

Also, ZFinish is the actual z-cordinate of the final cut and needs to be below ZStart. In your example, set this to -1.2.

Lastly, confirm that you've asked it to display all cut levels. Under the machining options, set ToolpathLayerShow to All. The default at the moment is just to show the top pass.

If anyone has suggestions on better, less ambiguous terminology to use I'd be extremely grateful. I'm new to cncing and need all the help I can get.

Thanks for taking the time to test this Sean. We'll beat this code into shape yet!

[andy55]

Can it import IGES files yet ?

What about different 3D machining operations ?

[ger21]

Originally Posted by 10bulls Now the distance mode is absolute but the I&J coordinates are incremental. Unfortunately now Mach3 can't read the file!

My Autocad macro outputs absolute code with incremental arcs, and it works fine in Mach2/3. Just change the G02/G03 mode in Config>State in Mach2/3

[10bulls]

Originally Posted by ger21 My Autocad macro outputs absolute code with incremental arcs, and it works fine in Mach2/3. Just change the G02/G03 mode in Config>State in Mach2/3

Thanks Gerry, that works a treat. Now the incremental.txt posted above looks OK in Mach3.
So I guess cambam needs 2 distance mode options. One for moves and another for arc centers.

[10bulls]

Originally Posted by andy55 Can it import IGES files yet ? What about different 3D machining operations ?

The priority at the moment is to get the machining side robust and easier to use which will include adding more operations (pocketing, drilling etc).

IGES support is on my TODO list, but will require quite substantial changes to the program as I'll need to introduce proper 3D geometric objects.

Once the machining side is more stable, the pace of development may slow down a bit as I'm hoping to start using the program for some projects I've put on hold while developing it.

[MrBean]

Hi 10Bulls,

I was intending to use CamBam to create the gcode for a stepper mount for my Mk2 "light table" conversion.
But I've come across a problem. I've attached a screen shot of the part in CamBam to give you some idea of what I'm talking about.

I made two 2,5d toolpaths, one for the internally cut regions and one for the external cut.

Because there are a few internal regions to cut, I ordered the cuts to "depth first" rather than "level", to save on rapid moves, back and forth. This should keep the machining time a bit lower.

Now the problem bit..... I need a stepover in the "width" of the cut to allow room for the cutter to pass the aluminium chips stuck inside the cut channel. I don't have any way of clearing them at the minute, unless I stand there and clear them manually.
I'm not sure if I explained that very well?? Anyway, because I have "Depth first" set. It cuts all z levels, raises the Z, and then steps over to make the cut wider, continuing to cut the Z levels again. This kind of defeats the object of having a cut wider than the cutter?

Although I have "depth first" set. It really needs to do the stepover part at each z increment (decrement?), continuing to full depth, and then move onto the next "inside region".

I'm not sure how well I've explained what I'm trying to say, so I hope it's not to gibberish.

BTW. It was a lot faster to get from "dfx to gcode", using CamBam than it was in Visualmill. Nice work.

Cheers, Terry.

[MrBean]

Wow. I received your email with the modified code. The part now looks like it should run just fine. I can still order regions by depth and have the stepover feature working, to allow plenty of room for the (cutter + chips) caught in the cut channel.

I also tested the custom file header feature you added. Inserting my G64 for CV mode. I see I can also use custom MOP headers too. Fantastic..... Now I can use CV mode for speed, where accuracy is not so important. And have "exact stop" (G61) mode for the close tolerance cut regions. This is a very nice feature. I can see that comming in very handy.

I think I'm going to nip out right now and start cutting my Alu stepper mount with the CamBam code.

All this ironed out in less than 24 hrs. That's dedication.

I think CamBam is ready to take it's place for all of my 2D profiling jobs, and once you've got pocketing sorted. That'll take care of all my 2.5D jobs too.

Great work, once again.

Thanks. Regards Terry...

[MrBean]

Okay. The machine's now running CamBams code as I type this. Cutting 5mm Alu.

Pictures of the finished part will follow tonight (unless it all goes wrong). Will be a while tho'. Cuts are shallow and slow. My bendy old CNC can't hack too much abuse when cutting Aluminium.

I'll keep you posted.

Regards Terry...

[10bulls]

In response to MrBean's thorough testing I have uploaded another bugfix release - beta 0.6C.

http://www.brusselsprout.org/CAMBAM/download.htm

As well as the depth first problem Terry spotted, this release also fixes a bug in the circle to polyline conversion. I was using 2 x 180 degree arcs, but this was obviously a bad idea and caused some problems with larger circles. I now use 3 x 120 degree arcs.

I've also added some custom gcode header and footer string options as well as headers and footers for each machine operation (for toolchanges, coolant etc). Hopefully this will reduce the amount of manual editting needed until I sort out a proper post-processor.
Multiple commands can be added with a | seperator denoting a new line.

One last change...The machining DistanceMode option (absolute/relative) now only applies to arc centers and does not affect moves or the G90/G91 codes. This is a quick, temporary bodge to get around some of the compatability issues mentioned in previous posts.

Originally Posted by MrBean I think CamBam is ready to take it's place for all of my 2D profiling jobs, and once you've got pocketing sorted. That'll take care of all my 2.5D jobs too.

It is very satisfying to hear that Terry. I am indebted to your enthusiasm and wise feedback and cambam is becoming a better program because of it.

[10bulls]

Originally Posted by MrBean Okay. The machine's now running CamBams code...

Woo hooo! I too have been doing a bit of cutting today, in acrylic which turned out fine.
One obvious missing feature I ran into was the inability to define the toolpath direction (climb,conventional,mixed). You can sort of change it by reversing the direction of the source geometry polyline, but it's a bit of a faff.