Drilling issue in my post

[DavidSV]

In my post for my horizontal, the drill cycles seem to not use the initial heights properly. Here is an example of the code I am getting:

 

T10 ( 3/8 2FL HSS CHAMFERMILL )

M6

T12

M8

G0 G90 G54.1P2 X.99 Y-.5 B0. S10000 M3

G43 H10 Z12.

G98 G81 X.99 Y-.5 Z6.3325 R6.52 F20.

Y-1.75

Y-3.

G94 G80

G0 Z12.

G54.1P1 X3.195 Y-.75 B0.

Z6.

G98 G81 X3.195 Y-.75 Z-.1075 R.025 F20.

Y-2.75

G94 G80

G0 Z6.

G54.1P3 X-.37 Y-.632 B0.

G98 G81 X-.37 Y-.632 Z-.59 R-.47 F20.

Y-2.868

G94 G80

G0 X-1. Y-1.313

G98 G81 X-1. Y-1.313 Z-.095 R.025 F20.

Y-2.188

G94 G80

G0 X-.37 Y-1.112

G98 G81 X-.37 Y-1.112 Z-.67 R-.47 F20.

Y-2.388

G94 G80

G0 Z6.

M9

G0 G30 G91 Z0 M19

G90

M01

 

My initial height is set at .25 incremental for the first drill cycle, and then at .25 absolute for the remaining drill cycles. When it goes from the P2 side to the P1 side it should rapid down to the initial height of .25 before it starts drilling. When I back plot this in Mastercam, it shows it happening as I would like, but in the machine it doesn't do that. Instead after it drills the hole, it lifts up to the 6" and moves to the next hole. When I have a bunch of holes on a side of a part its a lot of excessive rapid movements. Its getting the 6" from the reference points I have set in the home/ref. points page to move the tool out of the way when the machine indexes.

 

Does anyone have suggestions about where I should look?

 

Thanks

David

[K2csq7]

AFAIK the machine will rapid to the z value it saw on the G43 line in between holes then rapid down to the R and start feeding. Never changed work offsets between ops without forcing a toolchange.... maybe put a point toolpath down to Z1.0 between these two lines... then it will (should) only pop up to 1.0 between the holes.

Z6.
G98 G81 X3.195 Y-.75 Z-.1075 R.025 F20.

HTH

[Manuel0822]

Hope you figured it out already but if not here is a solution. I can see from the code that you may be using a Fanuc control on your machine.

 

The problem is the G98 call out you have on each drilling cycle. Fanuc & at least Haas controls uses G98 & G99 during canned drilling cycles. The difference between them is G98 will go back to the previous Z position, as Keith says, the one it read during the G43 line for your first face or "Z6." after your "B" axis indexing on the other toolpaths.

 

G99 on the other hand will only rapid out to the "R" position called out on your G81 line, so taking this portion of your sample code:

 

G54.1P1 X3.195 Y-.75 B0.

Z6.

G99 G81 X3.195 Y-.75 Z-.1075 R.025 F20.

Y-2.75

G94 G80

 

Notice how I replaced G98 by a G99, this way your machine will only rapid out to "Z.025" and then move to the the next hole as you wanted.

 

If you want Mastercam to do it for you when you post, then just check the Box "Use clearance only the start and end of operation", right under "clearance" box on your linking parameters tab during your toolpath definition.

 

I can see an scenario for using both G98 & G99, Let's say you were drilling on a part with pockets on and you have holes on both top face & at the bottom of the pockets, you would want to use G99 while you're outside the part but then use G98 for the holes on the bottom of the pockets just so you can avoid any walls that might be there between the pockets.

 

Anyways, this a long explanation for something so simple.