Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Tool length question


Greg_J
 Share

Recommended Posts

Hello,

I'm using a Integrex j-400 .

I have a part and I'm milling with the head at B90. and I need G43 P1 in my code.

How do I get MC to out put that code only when I'm using B90.? I looked through the misc. values and I didn't see any settings.

TIA,

Greg

Link to comment
Share on other sites
1 hour ago, Greg_J said:

Any idea why when the head is at B0 G43 works and then when I move the head at B90 G43 doesn't seem to be working?

I read the manual and it says that G43 B0 or just G43 for milling tools and G43 B1 for turning tools.

Something like I said you need to get a hold of your post supplier and let them help you sort it out. If the machine needs the code and your post is not supplying it then you need to get the post to understand the logic needed and get it corrected so you get the correct output needed to run the machine. Unless you send me the complete program and machine manuals and .z2g with everything could I even think about knowing where to start and what to do. You want to pay me for a day of my time to help you figure out I am all for it, but a simple call to your post supplier should take care of this pretty quickly and be free since it is not working correctly.

Link to comment
Share on other sites

Thanks Ron I appreciate the offer.

 

I did get it figured out with the help of David an AE at Mazak.

 

I needed a G68 Work Plane Shift in the program when ever you plan to machine on an angle different from the B angle the tool was measured on. I measured the tool at B0 and was running a program at B90.

In Mastercam under Misc. Values there was a check box for G68 Work Plane [0=OFF, 1=ON] and that fixed the problem.

 

Link to comment
Share on other sites
3 minutes ago, Greg_J said:

Thanks Ron I appreciate the offer.

 

I did get it figured out with the help of David an AE at Mazak.

 

I needed a G68 Work Plane Shift in the program when ever you plan to machine on an angle different from the B angle the tool was measured on. I measured the tool at B0 and was running a program at B90.

In Mastercam under Misc. Values there was a check box for G68 Work Plane [0=OFF, 1=ON] and that fixed the problem.

 

Thought there was an easy fix. Glad you sorted it out.

Link to comment
Share on other sites
17 hours ago, Greg_J said:

Thanks Ron I appreciate the offer.

 

I did get it figured out with the help of David an AE at Mazak.

 

I needed a G68 Work Plane Shift in the program when ever you plan to machine on an angle different from the B angle the tool was measured on. I measured the tool at B0 and was running a program at B90.

In Mastercam under Misc. Values there was a check box for G68 Work Plane [0=OFF, 1=ON] and that fixed the problem.

 

That seems odd, not saying it is wrong as I don't know enough to be sure... I programmed a chamfer path (odd shape where I really needed to control lead in/lead out etc) and just manually edited a B90. into the program and it drew correctly on the toolpath. Did not get a chance to verify it ran 'cuz a mazatrol guy got it done in Mazatrol....

Link to comment
Share on other sites

The verify did look good but when I put it in to the machine and simulated there it was out to lunch, the x and z were reversed and the tool length was applied to the tool at B0 not at B90. The tool went down near the chip conveyor, it needed the G68 X0 Y0 Z0 I0 J1 K0 R90.

Link to comment
Share on other sites
20 minutes ago, mikenaturalice said:

That seems odd, not saying it is wrong as I don't know enough to be sure... I programmed a chamfer path (odd shape where I really needed to control lead in/lead out etc) and just manually edited a B90. into the program and it drew correctly on the toolpath. Did not get a chance to verify it ran 'cuz a mazatrol guy got it done in Mazatrol....

I have seen exactly what he is describing on the Integrex and seen it other machines also. Fighting with an OKK right now that might need a software update.

Link to comment
Share on other sites

From an I machine

 

N23(CUT BAR FLATS)
G20 G10.9 X0
G91 G30 P4 X0.
G30 P4 Y0. Z0.
G0 G90 G53 B0.
M901
T23 M06
M200 
G97 S2037 M03
M108 M212 
G0 G90 G53 B90.
M107
G54
G68 X0. Y0. Z0. I0. J1. K0. R90.
G17
C90.
G90 G43 H23 X.4213 Z1.5
X.4213 Y.9003
M08
Z.66
G94 G1 Z.56 F30.
G3 Y.8497 J-.0253
G1 X.7106
G3 Y.9003 J.0253
X.7093 J-.0253
G1 X.42 Y.8855 F100.
G3 X.4213 Y.8348 I.0013 J-.0253 F30.
G1 X.7106
G3 Y.8855 J.0253
X.7093 J-.0253
G1 X.42 Y.8706 F100.
G3 X.4213 Y.82 I.0013 J-.0253 F30.
G1 X.7106
G3 Y.8707 J.0253
X.7093 Y.8706 J-.0253
G1 X.42 Y.8558 F100.
G3 X.4213 Y.8052 I.0013 J-.0253 F30.
G1 X.7106
 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...