cambam and Turbocnc

[wantsout]

Ive been trying to use cambam to convert dxf files to g-code, nothing fancy, a flower, a deer out line, and a few other files. and then was going to put them in turbocnc and run them to engrave them on a piece of 1/4" plywood. (Im just starting out so im reading all I can on this forum.) But the problems that im running into is when I convert the file in cambam,An error comes up in turbocnc and tells me that it needs both X and Y enteries with a G03 or G02 instruction.

Cambam doesent do this all the time or on every line of an arc instruction, so I want to know how to set the paramaters in either cambam or turbocnc to avoid this.

[10bulls]

Originally Posted by wantsout Cambam doesent do this all the time or on every line of an arc instruction, so I want to know how to set the paramaters in either cambam or turbocnc to avoid this.

I am not sure if this can behavior be changed in turbocnc.

I will make this an option in the next release of CamBam. I believe some CNC machines like TRAKs also insist on all axis variables for drilling ops too.

In the mean time, a work-around for this may be to change the ArcOutput (under machining options), to ConvertToLines, so only G00 and G01 moves are used. Hopefully turbocnc can cope with optional X,Y,Z values in G0/G1 moves?

[wantsout]

are you changing this in the turbocnc options or in the cambam options, because i cant seem to find those options in the turbocnc program. or the cambam options either. but you have to forgive me cause im slow. Im not sure what version of cambam Im trying to use so ill look it ver real good thanks for you reply

[wantsout]

Another Question, In cambam when I do the convert to g-code file and i look at it again in an editor it shows a G64 what is that code and what does it do I have looked for its definition every where but cant seem to find the answer. can any one help. I can find a G60 or a G62 but no G64

[10bulls]

The ArcOutput property is in CamBam. Click on machining on the tree on the left and look in the property grid.
ArcOutput = ConvertToLines will force all arcs to be replaced by line moves.

G64 is the code for constant velocity (or continuous) mode.
G61 is ExactStop mode.

Continuous mode is faster and smoother, but it can take shortcuts to preserve that smoothness. This can lead to inaccuracies, expecially when axis are driven with different ratios (leadscrew -vs-belt drive say). Oval shaped holes can be a symptom of this.

Exact stop, as the name suggests, ensures the toolpath hits all the control points so is more accurate but slower.

You can change these in the machining, options properties as well by changing the VelocityMode property.

[wantsout]

Thanks I found both places and changed both, now I will try another DXF file and see if this helps. You ppl are very helpful, but now Im trying to find out how to off set tool no. 2 so it will travel on the outside or inside as the case may be.

I want to route a line,circle,box or what ever with one bit then use another to decorate the same edge with another,but keep the part the same size..

[10bulls]

I have just uploaded a bugfix path, that may help turbocnc users.

It includes a new option that will force always outputting axis parameters (X,Y), for arc moves (G02/G03)

The link to the download and more information can be found here...

http://www.forum.cambam.org/index.php?topic=156.0

I have not tested this with turbocnc so would be interested to know if this helps.