help for mastercam post modification

[zafarsalam]

Hi all,

I need to modify the Mastercam 9 mill post MPHEID.pst for use with Heidenhain TNC145 controller. I have made a few changes myself and made it work to some extent. But all is by trial and error and still have to make changes manually sometimes to the output file. Anybody got experience with it? Have a better post to share?

Zafar

[millmore]

I have a similar problem. When I create toolpaths for a CNC router, each time Mastercam uses "G80" to can a drill cycle, it does not initiate a "G0" command before the next movement.

How can I get Mastercam to insert a "G0" automatically?

Thanks.

[Rekd]

Originally Posted by zafarsalam Hi all, I need to modify the Mastercam 9 mill post MPHEID.pst for use with Heidenhain TNC145 controller. I have made a few changes myself and made it work to some extent. But all is by trial and error and still have to make changes manually sometimes to the output file. Anybody got experience with it? Have a better post to share? Zafar

Be more specific to what you need. We can probably tell you how to do it.

[Rekd]

Originally Posted by millmore I have a similar problem. When I create toolpaths for a CNC router, each time Mastercam uses "G80" to can a drill cycle, it does not initiate a "G0" command before the next movement. How can I get Mastercam to insert a "G0" automatically? Thanks.

Find where you want the code inserted, likely inside the pcanceldc function.

pcanceldc       #Cancel canned drill cycle
      result = newfs (three, zinc)
      z = initht
      if cuttype = one, prv_zia = initht + (rotdia/two)
      else, prv_zia = initht
      pxyzcout
      !zabs, !zinc
      prv_gcode = zero
      if cool_zmove = yes & (nextop=1003 | (nextop=1011 & t<>abs(nexttool))), coolant = zero
      pbld, n, "G80", scoolant, e
      pbld, n, "G00", e
      if tapflg = 1 & stagetool <> 0, n, "G94", e # If tapping cycle, add G94
      tapflg = 0

Note the forth line from the bottom reads pbld, n, "G80", scoolant, e

That's where the G80 comes from. (One place anyway, there may be more in your post). I added a line below it pbld, n, "G00", e which will output a G00 on the next line.

(Back up your posts before you make changes, and when you make changes, only make one or two major changes at a time before testing it.

[millmore]

Thanks Matt,

I think this may work.

Before, when I would run a part without adding the G0, when the drill cycle was done, the tool would stay down in the material and take some random radius to the next point cutting material moving very slow.

To fix it, I would go in and add a "G0" on the next line bbefore the x, y, command ending up with something like this

From this...
******************

N130G99G81Z0.R.3F10.
N132X18.6668
N134G80
N138X.2489Y1.7052

******************
to this......
******************
N130G99G81Z0.R.3F10.
N132X18.6668
N134G80
N138G0X.2489Y1.7052

******************

That "G0" on line 138 is key.

When I use your method, I get this;

*************************
N130G99G81Z0.R.3F10.
N132X18.6668
N134G80
N136G00
N138X.2489Y1.7052
N140G99G81Z0.R.3F10.
N142X6.0668
N144G80
N146G00
N148X6.5489
**********************

Will this have the same effect?

Thanks.

[aperez]

Originally Posted by zafarsalam Hi all, I need to modify the Mastercam 9 mill post MPHEID.pst for use with Heidenhain TNC145 controller. I have made a few changes myself and made it work to some extent. But all is by trial and error and still have to make changes manually sometimes to the output file. Anybody got experience with it? Have a better post to share? Zafar

Zafar, I have the same problem. I'm trying to change the post to make it work for me. Send me a copy of your post. If we can't get help from others maybe we can work on it together.

Angel

[zafarsalam]

Originally Posted by aperez Zafar, I have the same problem. I'm trying to change the post to make it work for me. Send me a copy of your post. If we can't get help from others maybe we can work on it together. Angel

Angel,
What I have done is make three posts for profiling in x-y, y-z and z-x axis. And in Mastercam make sure you use 2d toolpaths (no helical paths or scallops). I couldn't make these posts to generate 3d lines. I triedbut couldn't upload those posts here. Mail me at (zafar at zafar dot com dot pk) and I will send the files to you.

Zafar

[mais202002]

Hi every one
i'm just new in this forum,very interesting reading cnc information post in here.
hope every one have a good day.

[Mike Stevenson]

Rekd's post change will work just fine. You do not need the G00 on the same line as your X and Y.

[oldjohn]

Hi Zafar and Angel
Did you fixed your posts?

John

[zafarsalam]

Thanks John for the concern. I have modified the post for my use and already made many parts using TNC145 control.

Zafar