CamBam PostProcessor?

Software / Firmware
1

Well, today I discovered cambam, and it is absolutely AWESOME. Seems much better than fusion for the kind of stuff I am doing. And a much better interface than estlcam. Here is the video I discovered it in:

I’m curious if anyone has used it successfully with the MPCNC? I think the gcode from the default postprocessor isn’t quite right so I may have to find one that works or make my own.

Vicious, it sounded like you had used it until the trial expired. I found a uh…less than legitimate way around that…feel free to PM me.

1 Like
2

Status Update:

So it looks like the only part of the gcode that was messed up that I can see was the starting code. The default postprocessor wasnt setting up home correctly at the beginning of the job. It worked when I replaced the start script with this:


N10 G90
N15 ;Units in mm
N20 G92 X0 Y0 Z0   <----- I THINK THIS IS THE KEY PART
N25 M84 S1800 ;Change Stepper disable timeout to 30 minutes
N30 G1 Z10 F2000 ; Lift Z 10mm to avoid dragging to first operation

It was originally this, which didn’t work right:

G21 G90 G64 G40
G0 Z3.0
( T0 : 3.175 )
T0 M6
3

Nice find.

When I used it I found one of the built in post processors actually worked as is, I have no idea which one it was but it worked fine. That is what I used in the first videos milling those purple faces in the HD foam. It used to have more features than ESTLCAM but I think it has them all now, like ramp into the cut and all that.

4

Oh okay well that is helpful. I will start the process of elimination then. That is easier than writing my own. I’ll figure out what works.

5

@Forest. Sorry to take so long to get back with you. I originally started using CamBam on a Harbor Freight milling machine that I converted to CNC. The MPCNC is way more fun though! I’m not sure that I always use a post-processor. I only used one when I added a laser and I needed a post-processor to turn the laser on and off. I had to define the laser pin in the Marlin firmware too in order for all of this to work. The only other thing is to change the syntax for gcode comments so that it will work with Marlin firmware too. I am attaching my Laser PP in case you want to see both how I turn the laser on/off and the revised gcode comment syntax.

Laser-255.txt (833 Bytes)

6

Hi,
I’ve been testing several different low cost CAM packages with my MPCNC:

EstlCam - I found a number of issues that for me make it a non-starter, and unfortunately didn’t get responses to my questions to assist with moving forward with the purchase. It seems to work for others so some of it is probably just being new to the CNC world. For the STL of my test model Estlcam produced junk for the gcode. Didn’t matter if I used the automatic 3D functionality or the manual process, didn’t produce anything close to the model.

CamBam - I’ve produced some accurate pieces in foam and really like a lot about CamBam. I did an initial test using the exact same STL file that I used with Estlcam test. CamBam produced something that was looking good, but I didn’t have something configured correctly so I stopped the test before it completed and switched over to using a DXF file and specifying Pocket and Profile operations. CamBam supports side profile operations which is nice. For fun I did a chamfer on one of my test holes and it milled perfectly. CamBam has a version that runs on Linux using Mono, and it looks pretty good. A couple of minor GUI issues, but non critical. CamBam is high on my list. $150US I need to revisit the STL test now that I’ve gotten more experience with CamBam and seen how MeshCam works. With CamBam I used the LinuxCNC post processor and it is working well with GRBL v0.9

MeshCam - Did a test using the same STL as with Estlcam and CamBam. Took the default rough and finish settings with my end mill for the tool. Was going to take a long time to complete and I forgot to add support tabs, so I stopped it before the final finishing run. But MeshCam generated gcode that appears to be perfect directly from the STL. The slot and rectangle pockets were properly milled, and the 8mm hole with 2mm chamfer from the model milled OK. As did a hexagon hole. I’m running another test with settings tweaked to add the support tabs and cutting the milling time in half, so I’ll know more when it completes. MeshCam, if more STL model file tests are good then MeshCam will probably move to the top of my list. $250US. Note: MeshCam can import DXF files but there is no way to specify pocket operations from the DXF. All holes go all the way though if you are importing DXF. Unlike with CamBam or Estlcam where you can specify outlines and then set the depth for each. So you have to use the STL files for 3D milling for sure. DXF is for people who wanted to do simple plates with holes in them according to the MeshCam forum. I used the ShapeOko post processor since that is GRBL based and it works well with GRBL 0.9 as well

FreeCAD - daily build Path Workbench. This is a CAM workbench for FreeCAD. It is integrating some of HeeksCNC processing into FreeCAD and it is coming along pretty well, and is usable for simple jobs. $0 so that is nice. Depending on the state of the nightly build there may be bugs, and as things change sometimes the docs and notes are not catching up. If I can free up some time I may help with debugging and adding features.

I wish that MeshCAM and CamBam had the same feature set, but then don’t so I’ll have to choose one of them. MeshCAM is a bit easier since it is more automatic, but if there are issues with the STL file that could impact the resulting gcode. CamBam has a good UI, and gives you a good amount of control. I don’t know yet if I could say that the 3D processing is good enough, but will be testing is some more over the next few days.

Both MeshCAM and CamBam have very responsive forums so that is a BIG plus when you need answers to questions about the software, or CNC in general.
MeshCAM is supposed to run under Linux using Wine and they have a web page dedicated to setting it up under Wine. As mentioned CamBam has a version that using Mono on Linux, and I have run some simple tests using that installation and it appears to work fine. I’ll be testing MeshCAM on Linux shortly as well.

I was able to get Estlcam to run on Linux using PlayOnLinux and making sure to add the libraries that are mentioned in another post on this forum. But as I mentioned other than simple DXF or SVG Pocket and Profile operations Estlcam just wasn’t going it for me. I always had to fight scaling issues, and in many cases Estlcam appeared to ignore the size set in the drawing file.

CamBam had no problem when the same DXF file was brought in. It got the size exactly right, and it was easy to set up Pocket and Profile operations, including the side profile one.

Has anyone else used CamBam or MeshCam lately, and if so what was your experience?

Burt

7

If I can ask, why are you doing STL models at all? I’ve 3D printed a bunch but I’m new to CNC – my understanding is that STL are 3D models, so unless you’re trying to mill a surface or something, how do you do tool paths with a 3D figure?

8

At the point mostly just looking at different possibilities.

While this isn’t a great example, since it would be better to use a “round over” bit for this, but in my test model I had a fillet(round over) on one vertical corner which will mill easily with 2.5D. But for additional testing and not having a round over bit handy I added a fillet on the left and rear top edge of the model. That’s where the 3D milling comes into play. Using an STL of my 3D model of my part I can pull that in and have it mill the round over using an end mill. Not saying that’s the best way to do it, but it does work.

Using CamBam I do a hybrid where I do the 3D Milling Operation just far enough down the part and then I have a second 2.5D MOP that finishes the profile milling the part out including having auto tabs to hold the part in place so it doesn’t rattle around in the stock and cause problems.

The other place where 3D milling is more likely to be used is to create molds for casting parts. My neighbor has been doing plastic casting for years building all sorts of interesting automatons that are quite lifelike. Doing 3D milling of a mold would allow taking a 3D model and milling a mold that can then be used with Latex or Resin casting. I’ll likely do some molds for him as I gain experience. CamBam has some nice features for producing molds from STL files.

But for 99% of my own projects I probably wouldn’t be using 3D milling. It was just a test to see how the capabilities of CamBam and the other packages I was looking at compared.

Burt

9

Hi mate, i know this was a long time ago, but i have just got my MPCNC working and have been trying to get some useable toolpaths out of Meshcam, bu t am having some trouble. How did you go about saving the code to be compatible with Marlin? Also were you still using Repeteir Host to run the file or something different? Thanks alot
Alex

10

Cambam:
The advice I got on the CamBam forum was to use the LinuxCNC postp, or the ISO plain gcode postp for Marlin based cnc’s. Not sold yet, as I have to test this. The PostP’s in Cambam use a different structure (XML) then most other cad/cam software, which is mostly text based

Up this thread someone asked why use STL’s. I use them for true 3d cnc carving quite a bit using Carveco as they are easy to import, and size in it. As I am looking for software, now 3 years into DIY CNC, that isn’t a rental, CamBam appears to be a contender at $150 USD (most cad/cam packages are rather pricey for perpetual licenses-$2k and up.

Now as I have a 4th axis rotary, Cambam has a plugin that is useful for making a flat stl out of a round STL, like a chess set, Unroll 3d Model. This produces a very good unwrapped flat model from the STL.

So, either I find a Marlin PostP, or just keep using CamBam as I have been, exporting stl, then back to Carveco for toolpaths.

BTW, there are many plugins for CamBam which would make it outperform EstCam, Carveco, Vcarve. Google it.