Live Tooling?

[*Jeff*]

Ideally, what level of lathe should I have to allow c-axis programming (live tooling)with the greatest of ease?

Currently we are running MCam V9 Lathe, & Mill level 1 & 2, however I am running into a problem when I try & tap (G32) on the x-axis, the tool motion seems to feed in correctly & the spindle stops & reverses, however on the (what should be feed out) it is rapiding out.

Can anyone tell me if this is a problem in the post processor or a mastercam issue? We are using a Haas SL-30 Big Bore Lathe.

Any help regarding these issues would be greatly appreciated.

Thanks, in advance.

Jeff

[P_Scott]

Jeff,

 

Mastercam's Lathe Tap operation does not have a Rapid Retract switch as most mill operations do. The MPLFan post tapping cycle for a Lathe tap (G32) should produce a feed in, stop spindle and reverse with a feed out. What is the version of Mastercam you are using and the post processor? Has the post been modified? Have you contacted your reseller about this issue? If it's a post issue, your reseller should be the one to help you modify it correctly. HTH

[PE @ IHS]

I have tapped using live tooling on several controls (not a Haas) and I have never seen the G32 command used for C axis tapping. On Fanuc, Seicos, and Mazak machines that I have run, you can use the G84 (milling) code for tapping with a live tool with success.

 

G32 does NOT contain a retract move. It simply synchronizes the 2 axis in motion with the spindle. This is used on main spindle tapping (on X0), and you generally need to input a spindle reversal command (M04) and feed out. On lathes that do not have a rigid tapping feature, you would need to use a floating tap holder for such work.

 

Tapping using live tools is different.

Try looking in the manual to see if your Haas takes milling codes for live tooling tapping operations.

 

Peter Eigler

[McRae]

Item 1-

Any level of milling will genereate toolpaths when bundled with Lathe. The complexity of the work will define what level of mill is required. For simple drilling/tapping and contouring/pocketing, stick with level 1. For some cool surfacing - go to level 3. Level 2 would give single surface capability but if you are going to do it - do it right (Buy it right or buy it twice...)

 

Item 2-

Peter E is correct. I specify a G84 type cycle when doing any Milling operations on the Mill/Turn centre.

 

1) Make sure that you select a Mill toolpath in the operations manager. Otherwise the machine will not distinguish between a lathe tapping operation (which would be a G32 in - Spindle Reverse - G32 out.)

 

2) That your post outputs the proper code. Know what you need before you ask the software to do it. This way you can assist/direct the post developer properly.

 

I have no opinion here on adding solids - perhaps Brian Davis has some insight.

 

[ 06-05-2002, 12:41 PM: Message edited by: MfgEng ]