Post help MC9 & X2 different result

[bogusmill]

We have converted an MC9 post for a BostoMatic 5 axis mill to MCX2 and get a different output. It's at the end of file and the MCX2 output is:

X10.Y10.R

 

What MC9 gave us, and what we want is:

X0.Y0.R

 

This is the part of the post outputting this code.

 

peof

# End of file for non-zerotool

n, "G01", "R M5M9"

n, xh, yh, "R"

n, "G49R"

n, "M2"

 

How do I get this to send my machine to X0. Y0. instead of X10. Y10.?

[Post dept]

Bogus, the xh and yh values are your home positions as you've set them up in mastercam. It looks as though your default home position in mastercam is X10, Y10 and will need to be reset in the last operation you're outputting to X0,Y0.

 

If you always want it to be X0,Y0, then you should hard code it in the post:

n, "X0", "Y0", "R" in v9

n$, "X0", "Y0", "R", e$ in X2

[Roger Martin from CNC Software]

There are a couple ways this can be handled...

 

1> You can set how how/where the system gets this ‘default home position’

or

2> If you always want X0Y0 you can alter the PST to force out the desired position.

 

Method #1 ->

 

In the Control Definition, under the Tool – Mill Topic page you’ll see a Default ‘home’ position option. You can set this to ‘Get position from the Machine Definition’ and they set the machine Definition values to 0,0. The home position values are defined in the Machine Definition under the Axis Combinations page.

(When you are look at your Machine Def. in the Machine Definition Manager, click on the “multi-arrow” icon to display the Axis Combo page.)

 

Method #2 ->

 

peof

# End of file for non-zerotool

n, "G01", "R M5M9"

xh = 0.0

yh = 0.0

n, xh, yh, "R"

n, "G49R"

n, "M2"

[bogusmill]

I may have to hard code it. Roger's method #1 hasn't worked. I had no trouble getting to the machine and control setting pages, and I set the default axis combinations for X, Y, Z, A, B to X0., Y0. Z10.0 (did not change Z) I'm still getting X10.Y10.R output. I did not close and reload MC. Will try that later when my helper doesn't have 2 instances of MC running.

[RObert TImby]

Bogusmill,

 

Look under your setting and open up the control difinition manager/ on the left side there is a control topic and click the "tool". look at the tool offset registers make sure they are at zero.

I had the same problem a while ago and that is where I found the problem at.

[bogusmill]

Your talking about the 2 offsets that have a default of 30? You have to change them to 0, and yes I checked to make sure they were set to 0 while I was there.

[Will Slota]

Bogusmill,

 

You are probably picking up the machine definitions home position. Click on machine definition manager, click yes when warned about editting your disk copy, when the machine definition manager opens click on the edit axis combinations button. The defaults for home position are probably all set to 10.0 I always set them to 0.0 for XY&Z. This should fix your output to be what you want.

 

Most of the default machine defintions seem to have a home postion set to X10.,Y10.,Z10. ...

 

Version 9 always output X0. Y0. probably because you never set it or checked the home position option and just never noticed it.

 

Hope this helps.