G99/G98 Warning

[Rick McAllister]

Happy Friday All,

 

I had a problem with my code not matching what I programmed.

 

The Scenario: Drilling holes on different Z planes. I chained points which were created at Z0 and Z-1.000 in a single operation.. I set the Clearance Plane at .1 Abs. Retract height at .1 Inc., Top of Stock at 0 Inc. and depth at - .75 Inc. The ‘use clearance only at start and end of operation’ was not selected. Backplot showed the tool retracting to the .1 Abs. clearance plane between all holes. Verify showed the same. Exactly what I wanted to clear an obstruction in the -1.000 pocket. The posted machine code was different. There was a G99 on the Z-1.000 holes which kept the tool down at Z-.900. This scrapped my part broke a tool and P.O. my set up guy.

 

If the Clearance Plane Height and the Retract Height are set at the same value a G99 is output regardless of ‘use clearance only at start and end of operation’ selection or Incremental setting. Also, Lets say you have .010 stock left on a surface and you retract is set at .09 Inc., .01+.09= .100 the same as the clearance plane, this will also output a G99 regardless of ‘use clearance only at start and end of operation’ selection.

 

BEWARE Mon Frere!

 

I placed a sample program on the FTP site called G99 G98 and Retract BUGs.MC9

 

If anyone wants to take a look I set up several ops with different settings. Posting with MPFAN will show the discrepancy.

[mayday]

Rick, had the same problem

I wiped out all output of G98, G99 from my post.

not worth the chance. I always retract to a safe clearance plane between holes. hey at 1000+ ipm at rapid traverse am i really losing any time??

not as much as when you crash and the operator goes

[Jammer™]

I've slammed a tap or two to depth at rapid feed because of this. All I do now, is use clearance height that is different from my retract height. (i.e. Clearance = .500 abs. Retract = .100 abs.)

This works for me now.

I wonder why them operators get so mad when you tap a 3/4-10 hole to depth at 800 ipm

[Hardmill]

quote:

---

I wonder why them operators get so mad when you tap a 3/4-10 hole to depth at 800 ipm

---

They're kind of touchy about stuff like that.

go figure

 

PEACE

[Thad]

Rick,

 

I can't exactly explain why it outputs a G98 or G99, but if you have a hole that resides at Z-1., and you give it a retract of incremental .1, MC did exactly what it was supposed to do by only going to Z-.9 (.1 incrementally above the hole). Although, I do think that should show up in verify.

 

Thad

 

[ 08-22-2003, 07:47 PM: Message edited by: Thad ]

[Rekd™]

quote:

---

Although, I do think that should show up in verify.

---

It can't be displayed in verify unless verify is keyed to the post. Everyone's posts treat drilling differently, so verify will just show the basic moves. No pecks, no dwells, no retracts etc. I don't know if it's possible or even worth while to make verify dependant on the active post. I can see much trouble with it set up like that.

 

'Rekd

[Rick McAllister]

Thad,

No it did not do exactly what it was supposed to do. I told it to feed at Z-.9 then retract to Z.1 abs. before going to the next hole. With the G99 output it did not retract above the part! Take a look at the sample I put on the FTP. Backplot it then post it. Take a look at the code. Do you have access to Vericut or another code verification program?

[Thad]

Maybe it only works that way for milling. Sorry.

 

Thad

[crazy^millman]

I have to agree with May^Day and like clearance plane but I have found with our post if you are doing different depth holes fr othe start that an incremental retract plane works the best wit hthis application and keeps that R vaule the correct way for drilling mulitplane holes. I have seen that and just do this as a way around any possible problems. I guess since we here make our programs, set them up, make the parts, and finish the parts we try to keep it from happening to us.

 

Crazy Millman

[Trevor Bailey]

+1000

 

Always when drilling at different depth, incremental.

[Rick McAllister]

Millman, May^Mayday,

 

Isn't it nice to have to modify a post to prevent something from happening that shouldn't happen in the first place. If only things did what they were told to do. In the next world maybe.

 

 

If it hurts when you do that, don't do that!

[mayday]

Rick,

back in the day when machines rapid traverse was 200 IPM on a fast machine G98/G99 was usefull. nowadays (is that a word?) I dont have a use for it. unless your parts have extremely deep pockets in it, but then again, why take a chance when you have to search the program for errors

[crazy^millman]

Well Rick I would look at it this way. We have four diffrerent machines here. I and another guy write programs for the machines we both do it different. If there was to be a perfect post for that perfect time for that perfect machine then why would they need us for. Doing this is not just about knowing Mastercam it also like it has been said in other thread a alot of different thing to do this and if you apporach with that then the little mods to the post are nothing but a bumb in the road of life.

 

Crazy Millman