cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Community Tip - Help us improve the PTC Community by taking this short Community Survey! X

No retract between holes when drilling

razmosis
11-Garnet

No retract between holes when drilling

Occasionally I encounter this problem with drilling sets of holes.  When creating a drill sequence of two or more holes, the path produced will drill the first hole, then without a Z move of any sort, it goes to the second hole's position.  The fix for it is to create multiple sequences rather than selecting multiple holes for the same sequence.  Most of the time everything goes as it should, but I can't trust that it will.

T1

M6

T1

S1030M3

G1G43X-.75Y-2.156Z1.F300.H1

G81X-.75Y-2.156Z-6.4231R.01F9.1

Y-1.356

G80

G1Z1.F300

M9

M5

G0G40Z3.0

G5P0

G28G91Z0

G49

G30

I prefer to see:

T1

M6

T1

S1030M3

G1G43X-.75Y-2.156Z1.F300.H1

G81X-.75Y-2.156Z-6.4231R.01F9.1

G80

G0Z1.

Y-1.356

G81X-.75Y-2.156Z-6.4231R.01F9.1

G80

G1Z1.F300

M9

M5

G0G40Z3.0

G5P0

G28G91Z0

G49

G30

I've ran this through a few different post processors and get the same result.  My guess is that it happens 1 in 20 times for me.  Usually a good operator catches it if I did not see it in the path before it got to them.  Curious if anyone else gets this issue?

Creo 2.0

Thanks,

Matt

1 ACCEPTED SOLUTION

Accepted Solutions

I've seen this kind of thing, too. Especially with reaming cycles for some reason. I think if you set CYCLE_OPTIMIZE to "NO", it may stop trying to be terribly efficient and instead go to the retract plane before moving to the next hole.

View solution in original post

6 REPLIES 6
SteveLucas
13-Aquamarine
(To:razmosis)

Matt,

I have seen it on occasion but I thought it might have been something I have done to cause it so I never have really looked into whether it's a post or Creo issue. Like you say my good operators catch it most of the time but every now and then they come in and look at you like what the hell did you forgot how to program a hole? That's what I hate!! I have to double check every time and that takes some time to do when there are a bunch of holes.

where I see issues like this the most is with copying sequences in a part program like where you have the same size hole on both sides of the same part. I see problems with drilling holes and chamfers not working as expected missing surfaces that were selected. in the case of chamfers even though I have deleted the first side references, Csys and retract and reselected the second side references.

Sorry no help in this post other than I feel your pain!

Steve

If you configure your post to input a G98 into the line G81 then you will get the result you are after. Looking at your program and the explanation of your issue on the machine. It looks like you have the setting G99 activated on your machine.

G99 will behave like you are explaining on your machine. The machine after drill each hole will only retract to the retract plane and then move to the next hole. Since your retract plane is R.01 the machine will only go .01" up in Z0 and then move to the next location.

G98 will make the machine go to the last Z position before the G81 cycle so in your case it will go to Z1. after drilling each hole and then moving to the next hole location.

If you input this in your machine the code below and do a dry run then you can see the actual Z1. retrace between each drilled hole. This is for all Fanuc controllers.

Also on your CNC machine if you look at what all the G codes that are active then see if the G99 is active on start up. G99 and G98 are modal until changed.

New with G98 option.

T1

M6

T1

S1030M3

G1G43X-.75Y-2.156Z1.F300.H1

G81G98X-.75Y-2.156Z-6.4231R.01F9.1

Y-1.356

G80

G1Z1.F300

M9

M5

G0G40Z3.0

G5P0

G28G91Z0

G49

G30

I've seen this kind of thing, too. Especially with reaming cycles for some reason. I think if you set CYCLE_OPTIMIZE to "NO", it may stop trying to be terribly efficient and instead go to the retract plane before moving to the next hole.

But the way his code is written, he is not telling the machine which code to be in. G99 is back to rapid plane, or G98 start plane. So the machine will behave with whatever is active in the controller.

Also if you want to pull the tool out farther to clear clamps or fixture. if you change your parameter "PULLOUT_DIST" to a value then the tool will also retract the amount after the drill cycle.

Thanks for the help, what I found to be the fix here is the cycle optimize parameter.

Top Tags