View Full Version : RhinoCam does not code MCS change

04-01-2012, 06:45 AM
Hi, I'm having trouble getting Rhinocam 1.0 to output code when making a change to the MCS during a milling operation to cut the face of a tooth on a 4 toothed wheel cutter M0.17 I'm making.

Below is the first few lines of the code where the MCS changes:

N86250 G01 X-0.2382
N86260 G01 Z0.6000 F114.0
N86270 G00 Z9.9622
N86280 (Set MCS 4)
N86290 (Parallel Finishing 4)
N86300 G00 Z3.2009
N86310 X-0.5739 Y0.0000
N86320 G01 Z2.6009 F57.0
N86330 G01 X-0.4304 Z2.6428 F76.0
N86340 G01 X-0.2870 Z2.6574
N86350 G01 X0.2870

There should be a rotate command for the A axis and the XYZ co-ordinates should also move to the new Cplane position, I don't think this code is doing that. There is no A axis code in the whole section!

Can anyone offer suggestions on what is going on? The Rhinocam simulation looks perfect but no code is generated for Mach3 to work with.

04-01-2012, 04:47 PM
just to add clarity, the Z axis is now rotated 128 deg, and the Y axis is +1.18, X axis 3.52 from the origin.

04-02-2012, 05:20 AM
I don't use this version of RhinoCAM (I just upgraded to 2012) but I'll give this a shot. My guess is that this is a postprocessor issue. See MecSoft Corporation User Forums (http://www.mecsoft.com/phpbb/viewtopic.php?f=7&t=2702)

First though, make sure you have the right variant of RhinOCAM. You do have one that is capable of indexed 5 axis work right?

To check what RhinoCAM is actually making of the MCS change you are programming, you can take a look at the APT-CL output. To do this change the post temporarily to APT-CL, post again and look at the output. If there are lines like this:


then this is not the problem - RhinoCAM is recognising and outputting your MCS change as well as the 5 axis movements you need.

Thereafter it is definitely your postprocessor that needs adjusting. Best way is to talk to Mecsoft.


04-02-2012, 06:24 AM
looks like the issue is Rhinocam, see below:

MOPNM/Parallel Finishing 4

Do you have any suggestions? Yes, I do have the 5 axis version, Setup is set to 4 Axis (only using 4). Thanks for your interest.

04-02-2012, 07:34 AM
The output you are getting shows that RhinoCAM has at least understood your MCS command. If you look at the output of the MSYS statement, it thinks you want the following:

local csys with:

origin at (1.173311,-3.518699,-3.677035)
rotation given by the matrix formed by the rest of the arguments, which I make -142 about the X axis

I imagine the 5AXANGS0, 5AXANGS1, ROT5AXIS and GOTO5AX are either from a different version of RhinoCAM or are only output in 5-axis mode. Either way they are slightly superfluous - RhinoCAM is identifying the new origin and rotation and outputting them as a matrix.

Maybe try the 5 axis mode? I only have a 4-axis machine but need to use 5 axis mode because my 4th axis is only the C axis. Therefore any aggregate tool I use has not only a C rotation, but also a (fixed) A/B rotation. But then again, I'm not sure what you're needing to achieve or what your setup is.

I still think this is a postprocessor issue though, and ultimately only Mecsoft will have the answer.

Best of luck

04-02-2012, 08:02 PM
Thanks Waywood, I'll try and run some code and test this out. How did you work out '-142 about the X axis' from that code I showed you?

04-03-2012, 06:21 AM

I don''t guarantee I have this right - these rotation matrices slightly fry the brain - but this is what I did:

The last 9 terms in the MSYS statement are a 3 x 3 matrix:


which correspond to a rotation about the X axis. These take the general form:

1, 0, 0
0, cosa, sina
0, -sina, cosa

(See Rotation Matrix -- from Wolfram MathWorld (http://mathworld.wolfram.com/RotationMatrix.html) equation #4)

-142 is just a matching arcsin and arccos between -180 and 180, which gives angle a.

04-03-2012, 08:01 AM
Thanks so much! I will give this a go myself! Using APT-CL output explains a lot about where unseen code is to be found - I could not see half of what I expected when I first generated a post.