Clearance in linking param NOT Working

[Rstewart]

X8 latest update fix

 

Fairly simple 4th axis indexing part.  This part is square, so I must use a high enough clearance plane in between Indexes as to not hit the part/tool.

 

All of the NON Drilling paths work correctly as the rapid to Z 3" absolute before index.

 

I've triple checked everything but i snapped a Spot drill....  

 

G80

M11

A180. X0. Y0.     Ain't gonna do it LOL

 

It Rapids to Z 3" AFTER index

 

Should I be using reference points  for even the simplest indexing tasks??

 

 

and please don't tell me I'm playing darts crazy millman

[Pilot Plant Supervisor]

You're using G98 Right?

[Rstewart]

Here Is my snippet of the Code.

 

I have Clearance of 3" checked in the linking param

 

Format:HTML Format Version:1.0 StartHTML: 165 EndHTML: 2394 StartFragment: 314 EndFragment: 2362 StartSelection: 314 EndSelection: 314

 

(OVERALL MAX: Z3.)(OVERALL MIN: Z-.4063)N10 G00 G17 G20 G40 G80 G90N15 G91 G28 Z0.N20 T4 ( 1/4 SPOTDRILL)N25 M6N30 (MAX: Z3.)N35 (MIN: Z1.5538)N40 M11 (UNLOCK)N45 G00 G17 G90 G56 A0. X0. Y0. S1375 M03N50 M10 (LOCK)N55 G43 H4 Z3. T9N60 M08N65 G94N70 G98 G82 Z1.5588 R1.6938 P100 F4.2N75 G80N80 M11 (UNLOCK)N85 A180. X0. Y0.N90 M10 (LOCK)N95 Z3.N100 G98 G82 Z1.5538 R1.6938 P100 F4.2N105 G80N110 M09N115 M05N120 G91 G28 Z0.N125 M01

 

[The Cathedral]

Make sure the box that says, "Only use clearance at start and end" is not checked. If that's not the problem, then it's a problem with your post. How do you get the index codes? Manual entry?

[Sticky]

You forgot to turn this option off:

 

 

 

 

This is a known bug, been this way for a long time. It is designed to wipe out spindles and tombstones. Gotta create jobs ya know.

 

http://www.emastercam.com/board/topic/77464-hmc-programming-training/page-2

 

http://www.emastercam.com/board/topic/76033-mpmaster-post-z-clearance-on-index-moves/

 

http://www.emastercam.com/board/topic/79507-clearance-in-linking-param-not-working/

 

There was another thread somewhere here where I complained about this and got jumped on for single blocking through all my clearance planes the first time I run a program because I never know when MC is gonna throw me a treat like this. They just suggested I run it and whip out that 25-50k for the spindle and tombstone when sh1t hits the fan :laughing: :laughing: :laughing:

[Sticky]

Make sure the box that says, "Only use clearance at start and end" is not checked. If that's not the problem, then it's a problem with your post. How do you get the index codes? Manual entry?

 

It is a Mastercam bug. You can get around this by modifying your post a couple different ways though, the first link above shows you how (thanks Collin!).

[Mike Whitten CAD/CAM Contractors]

The Z stops at Z3.00 on N55, since the drill cycle is in G98, the Z should return to the Initial plane of Z3.00 before index. This is providing that this is a standard Fanuc/Haas type of control. Am I missing something?

 

Thanks

[Rstewart]

The Z stops at Z3.00 on N55, since the drill cycle is in G98, the Z should return to the Initial plane of Z3.00 before index. This is providing that this is a standard Fanuc/Haas type of control. Am I missing something?

 

Thanks

 

 No, the cycle never returns to 3" before index.  MPMaster post and not using Any manual entry.  This is only happening on drill cycles with this file.

 

Thanks Sticky!

 

I can provide more info when I get back to work tomorrow. 

[Mike Whitten CAD/CAM Contractors]

Hello Rstewart,

 

I believe that if you start the drill cycle at Z3.00 and you are G98, the machine will definitely retract back to Z3.00. This would be on a standard Fanuc based controller.

 

What type of machine/control?

 

Thanks

[gcode]

The Z stops at Z3.00 on N55, since the drill cycle is in G98, the Z should return to the Initial plane of Z3.00 before index. This is providing that this is a standard Fanuc/Haas type of control. Am I missing something?

 

Thanks

 

This code would run safely on all our HBM's

It starts the drill cycle at a clearance plane of Z3.0,

runs the drill cycle

returns to Z3.

then indexes.

It's good code.

We've got a dozen Fanuc horizontals here and they would all run this code fine.

I don't think this is a bug or a post issue.

I believe there is a drill cycle parameter set to a non standard setting in the machine's control

 

you could add a  G00 Z3.0 before the index to prevent the crash, but all the Fanucs I've

got here don't need it.

[Rstewart]

This is on a 4 year old Mori Duravertical. Fanuc OiMD.

 

Why can't I Have a Z 3" after the G80???

[crazy^millman]

This is on a 4 year old Mori Duravertical. Fanuc OiMD.

 

Why can't I Have a Z 3" after the G80???

 

You can if you modify the post which is what Colin talked about in the other thread. I like others think it is not needed, but you are having problems so you adjust for the problem to eliminate that problem then that problem never comes back again.

 

Here is the direct link: http://www.emastercam.com/board/topic/77464-hmc-programming-training/?p=921501

 

HTH

[gcode]

This is on a 4 year old Mori Duravertical. Fanuc OiMD.

 

Why can't I Have a Z 3" after the G80???

 

 

you can edit your post to put a Z3. after the G80, but you shouldn't have to

 

Look up G98 in the fanuc manual..

 

The drill cycle should start at Z3.0 , drill holes at all the defined points cancel drilling at G80 and return to the Clearance plane  (Z3.0)

[Mike Whitten CAD/CAM Contractors]

 

 

I believe there is a drill cycle parameter set to a non standard setting in the machine's control

 Yes, I agree with gcode, look in the book under drill cycles and see if they list a parameter. This may be a wierd OiM thing. Ultimately, fixing the machine would be nicest, this way you won't have to modify posts forever.

 

Thanks,

[Sticky]

For G98 it should retract, but is still an MC bug because it does it with G99 too, which means crashy crashy time.

 

If you drill 2 or more holes it will output the clearance plane, if you only drill 1 hole ti doesn't output the clearance plane.

[gcode]

G99 just applies to the retract between hole locations

The machine should return to Z3. when it gets a G80 in G98 or G99

[slyym]

For G98 it should retract, but is still an MC bug because it does it with G99 too, which means crashy crashy time.

 

If you drill 2 or more holes it will output the clearance plane, if you only drill 1 hole ti doesn't output the clearance plane.

Not a bug! The G80 should make the machine retract back to 3", at least every machine i've ever used works that way. A G99 owuld only retract back to the R plane of R1.6938. Must be a different parameter setting but dont know which one.

[Sticky]

Not a bug! The G80 should make the machine retract back to 3", at least every machine i've ever used works that way. A G99 owuld only retract back to the R plane of R1.6938. Must be a different parameter setting but dont know which one.

 

Well apparently I'm not the only person that has run machines otherwise. I am gonna take a look at my parameter manuals. If MC isn't SUPPOSED to output the clearance plane, then why does it do it for 2 or more holes and not 1?

 

G99 just applies to the retract between hole locations

The machine should return to Z3. when it gets a G80 in G98 or G99

 

Hmm I will have to look into this, I have always coded the clearance plane at the end. MC does it for all hole counts over 1. I doubt that was accidental.

[Sticky]

G99 just applies to the retract between hole locations

The machine should return to Z3. when it gets a G80 in G98 or G99

 

 

I've gone and checked my programming manuals, all of them say that G99 is return to R only, G80 is cancel only. Which is what I thought.

 

I think you would have to create a custom G code (G80) to call the initial plane if you wanted to do this on the control. Which might not be a bad idea, but I don't recall ever having seen this done.

[Rstewart]

I'll try and making a "fake hole" to spot above the material tomorrow and see if I get a "Z" retract before index.

 

I will also give my dealer a call to talk to the app engineer.

[Sticky]

I've scoured my programming books and can't find ANY evidence of G99, or G80 initiating a return to initial plane for standard Fanuc controllers. I don't have complete information on how G code System A, B and C could affect this though.

[gcode]

I've scoured my programming books and can't find ANY evidence of G99, or G80 initiating a return to initial plane for standard Fanuc controllers. I don't have complete information on how G code System A, B and C could affect this though.

 

I couldn't either.

In fact I found an example that states you need a G98 at the last hole location to return to Clearance if you've been using G99

 

G0 Z3.

G99 G81 Z-1. R.1 F10.

X1

X2.

X3.

G98 X4.

G80

 

I even looked in the parameters book for settings that affect G98/G99 behavior

and found nothing.

 

That doesn't change the fact that every machine I've ever run rapids back to Clearance Plane at G80 in  G98 or G99 mode.

It has been nearly 15 years since I actually ran a machine so maybe my memory is getting foggy.

I don't ever use G99 in my programs these days

The operators at this shop are scared of G99 and no matter how safe or efficient my G99 tool path may be,

they're going to change it to G98.

 

It would be interesting if some guys would try this on different machines and post the results

[Rstewart]

I've looked at that PDF that Colin put together, and It's Exactly what I want

 

Now I just have to try and figure all that out, I'm not too versed in more than simple mods. 

 

Guess I'm not the only one who's machine doesn't automatically rapid back to initial plane after the G80....

[crazy^millman]

I've looked at that PDF that Colin put together, and It's Exactly what I want

 

Now I just have to try and figure all that out, I'm not too versed in more than simple mods. 

 

Guess I'm not the only one who's machine doesn't automatically rapid back to initial plane after the G80....

 

Bulls eye. Perfect throw and hit.     

[Sticky]

I couldn't either.

In fact I found an example that states you need a G98 at the last hole location to return to Clearance if you've been using G99

 

G0 Z3.

G99 G81 Z-1. R.1 F10.

X1

X2.

X3.

G98 X4.

G80

 

I even looked in the parameters book for settings that affect G98/G99 behavior

and found nothing.

 

That doesn't change the fact that every machine I've ever run rapids back to Clearance Plane at G80 in  G98 or G99 mode.

It has been nearly 15 years since I actually ran a machine so maybe my memory is getting foggy.

I don't ever use G99 in my programs these days

The operators at this shop are scared of G99 and no matter how safe or efficient my G99 tool path may be,

they're going to change it to G98.

 

It would be interesting if some guys would try this on different machines and post the results

 

It could be possible that the machines you were running, if they were setup by the same guy/company that someone created a custom user G80 for every control to always return to the initial plane. I would say that it is fairly unlikely but I think you could do it.

 

I think your memory is a bit foggy and you are just confusing G98 and G99. If you don't do a lot of hand coding or machine operation this would be very easy to overlook.

 

I've always put a value for a return plane when calling G80, regardless of which canned cycle I called earlier. I like redundant safety.

 

Mastercam also knows that you need to put the clearance value in when you call G80, because they do it anytime you drill more then one hole.

 

This is still a bug.

 

I know MC is loaded full of them but this should have been taken care of years ago.