Help with posting a G54

[rjoyner]

At work I use G54, G55 and so on in every program I run. I'm new to Mastercam and I can't seem to get Mastercam to put a work offset code (G54) in when I run my post. Can it be done, if so how?

[Rekd™]

What post, machine?

 

Yes it can be done, I do it via WCS, but there are many ways.

 

'Rekd

[crazy^millman]

if using the T/C Plane button Page then it is a Vaule kinda like this:

 

0=G54

1=G55

2=G56

etc

 

If doing it other ways then like Rekd said Post and Machine will help us to help you.

 

BTW(by the way)Welcome to the forum.

 

Crazy Millman

[iowajim62]

Hi rjoyner,

 

Like Rekd and Crazy said many ways.

 

But if you also tell us what Version of Mastercam as well as Mill or Lathe and what machine and post it will help alot.

Welcome to the Forum.

 

Also the Search function on this website is very handy for finding things like this.

[rjoyner]

I'm using Mastercam 9 with a HAASVF post for the HAAS mill.

[iowajim62]

Right on bro !

 

Go to Operations Manager and open any op.

Now click on parameters right below the name of the op you opened. Next click on T/C Plane button, now click on the lower left button where it says Work offset and put "0" for G54, "1" for G55 etc.

 

Remember this is just "my" way of gettin u goin.

Ur reseller can help u setup ur post if u wanna get fancy.

Also the other folks in here will have some ideas.

HTH

[rjoyner]

I did that and it said "THIS FEATURE IS NOT SUPPORTED BY YOUR PROCESSOR (SEE NUMBERED QUESTIONS 161-167 IN YOUR POST).

 

What does the mean?

[crazy^millman]

Make sure this part of the post says This:

 

code:

---

161. Enable Home Position button? y

162. Enable Reference Point button? y

163. Enable Misc. Values button? y

164. Enable Rotary Axis button? n

165. Enable Tool Plane button? y

166. Enable Construction Plane button? y

167. Enable Tool Display button? y

168. Check tplane during automatic work origin creation? y

---

Should be a cake walk from there unless you need to change this also:

code:

---

 force_wcs   : no    #Force WCS output at every toolchange? 

---

Then that should take care of you unless you are going to be doing 4th axis work then say yes to that button.

 

Crazy Millman

 

Also what is the Date on the Post you are using?

 

[ 12-01-2003, 08:10 PM: Message edited by: Millman^Crazy ]

[Chris Rizzo]

I made a slight mod to my Haas post...In the t/c plane toggle instead of inputting 1,2,3,4 etc, and having the post tranlate them into 54,55,56,57, I now just directly enter the number that I want to post. If I want 59, I put in "59"! not "6". . Let me know if you want that mod, and I'll dig it up.

[crazy^millman]

CMR I went A step futher since I have G154 Pxx 1-99 I changed my post to output to soemthing like this:

 

1=G154.1 P1

2=G154.1 P2

etc...

 

Though the G54.1 will work also just depends of how you have the parameters set up is all.

 

Crazy Millman

[CAM Disciple]

Try turn on your misc integer 1 to 2.

 

Also, find out if you have this section in your post:

 

code:

---

pwcs #G54+ coordinate setting at toolchange

if mi1 > one,

[

sav_frc_wcs = force_wcs

if sub_level, force_wcs = zero

if workofs <> prv_workofs | (force_wcs & toolchng),

[

if workofs < 6,

[

g_wcs = workofs + 54

]

else,

[

g_wcs = workofs + 104

]

if workofs >= 0 & workofs <= 25, *g_wcs

else, "ERROR - Invalid Work Coordinate System", e

]

force_wcs = sav_frc_wcs

!workofs

]

---

If you have this section of code in your post, turning on mi1 to 2 will enable otputting the WCS.

 

Make sure you call out pwcs in tool change or null tool change section.

 

If you still having problem posting wcs, try finding all the pwcs section in your post and paste it in this thread. We might be able to help you out.

[crazy^millman]

See why I like this place you may not have the answer but soemone will put it up there for you if it is possible. Thanks for that sharing CAM Disciple very cool.

 

 

Crazy Millman