stock recognition

[Thoob]

Hi, I'm using Lathe X4 and I sometimes can't enable my stock recognition in my toolpath properties. I don't know if its something I'm doing or just random but sometimes I can select the adjust stock button and sometimes its grayed out where I cannot select it. When its grayed out, it always tries to take everything in one cut even though I'm in a rough cycle with .05 DOC. Any ideas?

[gcode]

typically, this happens if you don't have stock properly defined.

[Thoob]

Ok, I have the stock set up like this. Its on cylinder for geometry. It has a 3"OD, 0"ID and 15" length. I am using a drill to drill a 1" hole, then using that same drill to bore the hole to 1.25. (Its an Insert Drill). The drill seems to go no problem, but the bore part has stock recognition grayed out and it wants to take it all in one cut. I tried changing my stock to have a 1" ID but its still the same. Could it be anything with how my geometry is drawn?

[Sbarner]

I think it has to do with the fact that you're using an insert drill to bore with. IIRC, I had this same problem, so I had to draw the drill/insert and define it as a boring bar...I think. I'm at home now, but I can look tomorrow at work.

[Sbarner]

I checked. I have the same drill defined twice. Once as a drill, once as a boring bar. That took care of the issues. I hope we see some support for inserted drills soon.

[Thoob]

So I just need to define it as a boring bar then eh? Ya thats weird that it doesn't have that support. Thanks a lot. I'm going to go try it out.

[Thoob]

I tried that. It works now. I would have been fighting that forever had you not mentioned it. Thanks Steve.

 

***Edit*** When I define the same tool number as a boring bar, the numbers don't add up in my control.Example when I post the program, the drill enters at X0 but then when it starts to cut, it is at 1.1 on X. This is ok if its an actual bar but because in my offsets, its calculated as X0, I would need the program to cut at X.1, not 1.1. Hope that makes sense. Anyway, would I have to teach all my insert drills like a boring bar and have the program cut at X1.0 instead of X0? Or is there other ways. I don't prefer it this way because the verify is not right.

 

[ 09-20-2010, 08:56 PM: Message edited by: Thoob ]

[jhjr]

You could use a different offset at the control for the boring operation. Example use T0707 for drilling and T0777 for boring. It's a pain but verify would be right. HTH

[Sbarner]

Thoob,

 

Jim nailed it. You have to use a different offset. I think when we did it here, the drill was T404, and the boring op was T0414. So then T404 is setup as you would a drill, and T414 is setup like a boring bar. Make sense?

[Mike S @ S4A]

The issue is related to tool profile and how it is compensated differently (Z only for drilling,

D or ID and Z for profiling/facing). If Mastercam is sharing one common geometry file for the tool you have to be careful. Better to have separate profiles saved for the insert drill as a drill and as a boring bar, Then reference those in the Mastercam ops/tool manager. Its also helpful to lock the drilling op that's calling, say, T0202 for drilling before creating a boring op with T0220 (same tool in the actual turret calling both D and Z compensation.

Only serves to emphasize the value of good training and tech support.

[Thoob]

Ok, thanks a lot fellas. I will do just that.