How to get a G98 to post

[StoneyNH]

All my drilling cycles post a G99.Theres times when I want a G98 instead.How do I get it to post a G98 drilling cycle?

 

Im using MCAM X4.

[The Cathedral]

IIRC there was a thread about this not too long ago. What post/machine def. are you using?

[StoneyNH]

Im using a post that was made for the HAAS machine.Its the only one I can find.If I could find the HAAS generic post I could compare the 2 to see whats different.Do you know where I could find the HAAS generic post?

 

And do you know how to use file compare to find the difference?

[neurosis]

I have to ask the obvious -

 

In your <linking parameters> do you have "use clearance only at the start and end of an operation" checked?

[StoneyNH]

When I want to post a G98,No,I have it unchecked,its my understanding that's whats supposed to make the difference but it doesn't.So Im thinking in the post I use we must have missed what makes it do that.

[THEE THAINZ™]

Do you have the check box next to clearance checked? It needs to be for it to post the G98.

[Guest]

a z2g may help but just not sure how many people still have X4 installed......

 

I do at home and not really sure why :headscratch:

[StoneyNH]

Yep,the check box next to clearance is checked,its the one underneath it I have unchecked,the use clearance only at start & end of operation.

[Mgrenier]

You might want to check these 2 lines in your post (they are from the generic Haas post):

 

sg98    : "G98"      #Reference at initht

sg99    : "G99"      #Reference at refht     

sgdrlref : ""        #Target string

 

HTH,

[StoneyNH]

When I try to lookup my posts,Im opening Files in my toolpath manager,clicking on edit in machine section,the only post in Post-processor is my MPHAAS_rev4.PST.Shouldnt I be able to find the generic HAAS post in there as well?

 

How do I open my post to see whats in it? I cant figure that one out.

[Mgrenier]

You post are in the shared mcamX? folder (C:\Users\Public\Documents\shared mcamx?\mill\posts)

 

They are text files, just open them with any text editor.

 

HTH

[Allan]

Un-check the Clearance or use the use "use clearance only at the start and end of an operation" then it will output the G98 (return to R plane).

 

 

[StoneyNH]

Allan been there done that,it doesn't work.Trying to figure out what I gotta do to get it to work.

[Mgrenier]

Like was mentionned before,

 

Create a z2g file to share or at least screen shots of your operation settings in mastercam.

[StoneyNH]

Yep,I saw John mentioned that,but that's way over my abilities & understanding.Is it something I can do with minimal knowledge? If so,how do I go about it?

[Mgrenier]

To create a z2G file go to Help -> Zip2go utility

 

Make sure to add the post file in you z2g.

[Guest]

Here's a quick video on making a useable z2g

 

Make sure you file is saved first, then.....

 

[MIL-TFP-41]

Are you using the same values for your retract height and clearance height?

 

If both are set to absolute and both are set at .1 for example then you could get a G99.

 

Set the Clearance at .1 and Retract at .05 and you will get a G98.

 

This stuff is post dependent, so some will behave different than others.

[StoneyNH]

Want to thank everyone that chimed in & had something to say.I gathered enough information to relate to my IT guy, to explain what I was trying to do.He found the post & modified it so it does what I want it to.Now I can post G98's without having to edit them manually.It was everybodys comments that helped get it done.-THANX-

[Rstewart]

I gathered enough information to relate to my IT guy, to explain what I was trying to do.He found the post & modified it so it does what I want it to.

 

 

Your IT guy can write / Modify posts?!?!?

 

That's a pretty sweet deal

[StoneyNH]

Well our IT guy understands all this computer lingo better than me & its his job to keep everybodys computer running efficiently,so I guess Im lucky to have him around.

[cncfrank]

If your running it on a Haas, our Haas's automatically use G98, and the previous programmer never used G98 or G99.  So I found out the hard way when I ran a job using G99, the machine Kept it, and when the operator ran the next job that didn't specify G98 it didn't jump when it normally would........I take them all out of my programs now.

[Sticky]

If your running it on a Haas, our Haas's automatically use G98, and the previous programmer never used G98 or G99.  So I found out the hard way when I ran a job using G99, the machine Kept it, and when the operator ran the next job that didn't specify G98 it didn't jump when it normally would........I take them all out of my programs now.

 

On a Haas, and many other controls, G98 and G99 are modal, so they will stay active until you power the machine down OR command otherwise.

 

It's good practice to ALWAYS add G99 or G98 to any canned cycle call. Leave nothing to chance...