Drill depth - A2100

[dourk]

On my A2100 controls, they automatically account for the drill tip angle in the drill depth (if I program a 1" hole, .500 deep, it will actually go ~.800 deep).

 

Is there some way to compensate for this in MC lathe? Here's why...

 

Programming a bore that is .625 deep. I need the full dia of the drill .650 deep. If I add drill tip comp in MC, everything looks good, but then I drill to deep on the machine. If I program it knowing the machine will go farther, then when I run the bore in the drilled hole, the backplot shows the bore digging into undrilled material.

 

Usually I'll turn on drill tip comp while programming, then turn it off before I post. But, that's a pain.

[Barghest]

I dont know anything about your controll but have you checked to see if there is a parameter at the machine to turn the tip comp off.

[dourk]

Sure, I can turn it off. But I like it there. Too many jobs are in production to change it. And when I'm programming a quickie at the machine, I don't have to do any figuring out to get my drill to the right depth before I tap it.

[Noel]

Mabey there is a parameter in the machine for drill tip angle that you could set to 180 so that it would drill no deeper than the programed depth.

 

Noel

 

 

[Guest CNC Apps Guy 1]

Give Noel a cigar!!!

 

There is s parameter in the control for Auto Tip angle compensation.

 

[$CYCLE_PARAMS(2)HOLE_DEPTH]=2

 

The value should be 2 which is no comp I believe.

[Noel]

What kind of cigar?

 

 

Noel

[dourk]

But, I WANT the comp in the machine. It's handy to have.

 

And I don't want to edit the > 300 programs that already use it.

 

I want mastercam to operate the way I do, not the other way.

 

I'm thinking maybe put something in the post so that I can have drill comp on, then the post reverts to the depth without the comp.

[Harryman]

Change the MC definition of the drill to 180 point???

[Guest CNC Apps Guy 1]

That's fine, you can turn tip comp off in Mastercam and set the machine parameter to comp for the angle in the tool page at the control. Personally i HATE it because I want control of the toolpath in Mastercam NOT at some piece of garbage control that freaks out when the weather gets too hot, or when the power surges, or when a brownout occurs. My Mori's don;t even skip a beat unless the power goes OUT, but that's another story.

 

Go into Mastercam's COnfig, go to the NC Settings Tab, go to the Operations Defaults, click save and an Operation's manager pops up with all the toolpaths in it. Go to the drilling cycle and turn off the tip comp or however you want to change it. Exit, save and continue working..

[dourk]

Harryman - that's about the simplest idea. Perfect. Thanks.

 

James -I have no problem with the A2100 control, other than the fact that it's soooo damn slow. Forever to boot. Forever to swap screens, etc. It has a ~lot~ of nice features that oughta be in other (fanuc/yasnac) controls in this day and age.

 

What I hate it the absolute junk iron it's bolted to. Cinci arrows/sabres are the flimsiest, weakest, unreliable machines I've ever used.

[crazy^millman]

brett tell us how you really feel

 

All I got to say about that.

[Roger Peterson]

Well nobody ever accused fanuc controls of being feature laden... Why is it you were using drill tip comp in the control, written by hand? Is this something you could turn on and off via Gcode with a macro? If so turn it off at the start of your new programs generated with mastercam and turn it on in old programs. I kind of agree with James, I want the machine to do exactly what the gcode tells it, not it's interpretations which can change with the barrometric pressure and the position of the moon. I know a few guys that have attended a support group for the A2100 and I'll ask them.

 

 

HTH and good luck

[Guest CNC Apps Guy 1]

quote:

---

...Is this something you could turn on and off via Gcode with a macro?

---

Yes. [$CYCLE_PARAMS(2)HOLE_DEPTH]=2 will allow you this control. Not sure if the control will accept it without a reboot. You know how those temermental PC's are.

 

quote:

---

...support group for the A2100...

---

Do they gather round in a circle and comiserate(sp?) on what a poor machine tool purchase decision they made???

 

James teh thank you sir may I have another, thank you sir may I have another...

[Roger Peterson]

That's what I was afraid of, it doesn't do him much good if has to reboot. No comment on the support group... And out in cali the tide could also affect the A2100.

[steve f]

brettj,

 

if you know how to tackle it in the post, you could try creating logic that would reverse calculate drill tip comp and subtract it from the actual drill depth. That way your 1" drill - .500 deep would actually be programed as Z-.300 so the control comp will send it 1/2" deep.

 

steve

[dourk]

steve,

 

I was thinking the same thing, but is there a way for the post to know if the 'drill tip comp' box was checked on the operation page?

 

That way I could account for both conditions.

[Guest CNC Apps Guy 1]

Here's the drilling parameters you can use.

 

quote:

---

OPS: PRM_DRILL

10100 Drill cycle

10108 First peck increment

10109 Subsequent peck increment

10110 Peck clearance

10111 Retraction distance for chip break

10112 Dwell

10118 Pre-defined bore shift

10117 Add this amount to total depth

10115 Adjust depth per drill tip (True/False)

 

12018 Drill point sorting method used

15071 Custom drill cycle parameters

15072 Custom drill cycle parameters

15073 Custom drill cycle parameters

15074 Custom drill cycle parameters

15075 Custom drill cycle parameters

15076 Custom drill cycle parameters

15077 Custom drill cycle parameters

15078 Custom drill cycle parameters

15079 Custom drill cycle parameters

15080 Custom drill cycle parameters

15081 Use custom parameters is checked (True/False)

 

12019 Drill5ax output format axis type selected: 0=3 axis, 1=4 axis, 2=5 axis

 

12020 Use points and lines or points

12021 Tool axis option

12022 Tip position control

12023 Project type (to plane or surface)

12024 5-axis tool display length

12025 Drill5ax output format 4-axis type axis selected (0 = X, 1 = Y, 2 = Z)

 

12254 Plane vector for drill5ax plane option 12255 Plane vector for drill5ax plane option 12256 Plane vector for drill5ax plane option 15212 Output 1018 NCI (sub program) line in drill cycle (True/False)

 

15213 Subprogram output mode: true = incremental, false = absolute

---

Taken from Mastercam Version 9.1 MP Post Processor Reference Guide 7-111 Volume 3 Chapter 7

 

It is available through your reseller. I would STRONGLY reccommend getting it if you plan on doing ANY post processor customization.

 

HTH