Hi :)
I'm new to CNC so I'm using Cambam to create text to engrave on aluminum plate and also I'm interested in engraving a pic on the same material.
I have a dxf file that a friend made for me, from a pic I've worked. I am able to open it in Cambam, but at the moment I try to create a Gcode from it, Cambam stop working (Not responding) and I have to close it. I am using the free version 0.8.2.
To create the Gcode I select the entire graphic, then go to CAM and select "Engrave"; then right-click on Machining from the tree and select "Create Gcode". At that point nothing will happen.
Can somebodie please tell me what is that I'm missing or how to do it?
Thanks al lot.

Hi Josh,

The dxf opened in cambam ok but when i tried to convert to polyline ( the outside of the face) cambam hung. When i treied the same thing in a little line near the ear it converted ok. I think it could be to do with the dxf. Autocad would not open it. At the end of the day post this issue to http://www.cambam.co.uk/forum/ I am sure youy will get a quick and accurate response form iobulls (Andy) or someone more knowegable than myself.

Paul

Hello there!

This is quite a complicated drawing made up of many splines.
Under Tools - Options, there is a setting called SplineToPolylineTolerance.
Unfortunately in the free version, there is a bug where this setting is being ignored and a much lower tolerance is being used which causes the spline to be converted to an excessively large number of small segments. This takes ages and is why CamBam is not responding.

This bug was fixed in the plus versions of CamBam. I just opened your file in the latest 0.9.6e release (http://www.cambam.co.uk/download/untested/cambam-plus-beta-release-096.html) and set
SplineToPolylineTolerance=0.1. Generating the toolpath took a couple of minutes but worked fine.

The time is taken converting the Spline objects to polylines (straight segments and circular arcs). I converted the splines to Polylines manually (CTRL+A, then CTRL+P). This took the minute or so to convert, but now the engraving toolpath generation is practically instant.

Feel free to try this in the plus release yourself as you will get 40 free evalutation sessions. The plus version has moved on a lot from the last free version.

I have attached the CamBam file that I converted splines to Polylines. This was generated in the plus version but seems to load fine in CamBam free. I also exported the polylines to a .DXF file (interestingly this is less than 1/3rd the size of your original spline file).

I hope all this helps and good luck with your engraving.


Hi :)
I'm new to CNC so I'm using Cambam to create text to engrave on aluminum plate and also I'm interested in engraving a pic on the same material.
I have a dxf file that a friend made for me, from a pic I've worked. I am able to open it in Cambam, but at the moment I try to create a Gcode from it, Cambam stop working (Not responding) and I have to close it. I am using the free version 0.8.2.
To create the Gcode I select the entire graphic, then go to CAM and select "Engrave"; then right-click on Machining from the tree and select "Create Gcode". At that point nothing will happen.
Can somebodie please tell me what is that I'm missing or how to do it?
Thanks al lot.

Thanks, Andy :)
Both dxf files open fine in my Cambam. No problem. Even the previous dxf that I sent you guys. What you did solved the problem creating the Gcode. Cambam creates the Gcodes now, but maybe there is still a problem with the code because it does not recreate the image in CNC Simulator. What I get is lines and circles with no sense at all. There is something wrong still and I will download that version of Cambam to generate the Gcode from those dxf files you've sent to me.
I'll keep you posted.
Thanks again, Andy :)

...Cambam creates the Gcodes now, but maybe there is still a problem with the code because it does not recreate the image in CNC Simulator. What I get is lines and circles with no sense at all.

Sounds like your next problem is Arc center modes.
Arc g-code moves (G02,G03) have an I and J parameter, which is the centre point of the arc. This can be an absolute coordinate, or relative to the first arc X & Y coordinates.
In CamBam, if you click on the Machining folder, you will see a property called ArcCenterMode which you can set to Absolute or Incremental.
There is no real standard which it should be, but it needs to be the same setting in your simulator and CNC controlling software, otherwise the arcs go pretty crazy or you'll get errors reported.

There are corresponding options in most CNC controller software or simulators. Make sure they are all set to the same setting.

Sounds like you're nearly there! :)

Hi, Andy :)
Sorry I couldn't say the following before. My machine and computer are at the basement and I was getting late to go to work (where I am now), but just before I left home ( to be late at work, of course) I went to the basement and I tried to open the Gcode generated from your dxf in Mach3. Amazingly it oppened:banana:
Then what followed was scarry: I sent it to engrave and the machine went crazy. Thanks God to that "Stop" button on Mach3 :)
Conclusion: the free Cambamn seems to be able to create the Gcode if you do what you did to the dxf created by my friend in ArtCam. The other thing is that I have to review the file size. I thing that's what happend with my machine and the Gcode. It is too big for my 16x12 bed.
I'll take a second look at it and I'll let you guys know.
Seeya :)


Sounds like your next problem is Arc center modes.
Arc g-code moves (G02,G03) have an I and J parameter, which is the centre point of the arc. This can be an absolute coordinate, or relative to the first arc X & Y coordinates.
In CamBam, if you click on the Machining folder, you will see a property called ArcCenterMode which you can set to Absolute or Incremental.
There is no real standard which it should be, but it needs to be the same setting in your simulator and CNC controlling software, otherwise the arcs go pretty crazy or you'll get errors reported.

There are corresponding options in most CNC controller software or simulators. Make sure they are all set to the same setting.

Sounds like you're nearly there! :)