O/T: Another Integrex Question

[RStuart]

Is anyone familiar with thread milling on this machine? Is it possible to do thid in Mazatrol or do I need to do it in EIA/ISO? Thanks in advance.

[crazy^millman]

I did it with Mazatrol but that was in 3 axis so not sure if it would work if doing it 5 axis mode. If I were doing it 5 axis mode think I would rather do it EIA to know exactly where the tool is going unless you use the Mazatrol TPC for your apporcah and retract points. Just my humble opinion is all.

 

HTH

[PE @ IHS]

You can't do it with Mazatrol, except by using the manual G code option within Mazatrol.

 

There is no such thing as threadmilling in 5 axis mode.

[crazy^millman]

Well yes you can you use the helical circle milling and cheat your way through it. If ememory serves me correct I use to use the TPC for the start at 0,0 or where every the center of the hole was and then I would use 0,0 for the end then I would use the Z point above the start if that was .25 then that was my start and end Z for doign that operation. It is was quirky at best but did work.

 

quote:

---

There is no such thing as threadmilling in 5 axis mode.

---

You mean in Mazatrol right becuase you can do this in 5 axis with Mastercam and EIA. The example of this is Called CRAZY_5AXIS_THREAD in the Mc9 folder on the FTP.

[Harryman]

Circle mill tornado = 1. Set helix pitch = thread pitch. Set hole OD = thread OD. Outside to inside direction only. Right hand screw = right hand helix. Will be conventional milling. It will work with B axis at angles other than zero or 90. Do the math carefully for start points. HTH

 

Sorry for slow reply, been super busy.

[crazy^millman]

Thanks Harry Torando Knew it was something like that has been a few years I appericate the response.

[PE @ IHS]

You are right Harry. The tornado option wasn't present when I used to have a real job a few years back.

 

Ron, I was talking about 5 axis motion, not 3 axis motion tilted in A or B. You are right about the WPC, it can be set at any plane and threadmill in a locked (3 axis) position.

[chris m]

HIJACK

 

Hey Harry:

 

What spindle do you have in that new Integrex; Capto or KM?

 

If its Capto I have some tools I can sell ya...

 

C

[RStuart]

I had tried it in tornado milling. I knew that much. The only problem is in tornado milling it does that darnred finish pass at the final depth at a constant depth, which in turn ruins my threads. How do I get rid of that finish pass at the end?

[McRae]

The only problem is in tornado milling it does that darnred finish pass at the final depth at a constant depth, which in turn ruins my threads.

 

Though catastrophic to the feature being created - this is absolutly funny! The "Macro" is actually made for helical with a button tool for roughing a bore where a clean up pass at final depth is needed for a blind bore. I can't get my Pro/E system to create this move at the end of a cycle and you can't get the Integrex to keep from making it!

 

Call national applications in KY and ask for the software depatment - you have a seriuos question on the this and Mazak has lifetime service/assistance that they offer with their machines.

[chris m]

quote:

---

Call national applications in KY and ask for the software depatment - you have a seriuos question on the this and Mazak has lifetime service/assistance that they offer with their machines.

---

Yeah, lemme know how you make out with that...

 

Chris teh how Mazak got to be the biggest machine tool builder in the world I'll NEVER understand...

[Harryman]

Use a single point tool and the cleanup pass won't wreck the part. A threadmill does you no good anyway since all cutting is done with one tooth as the helix runs outside to inside.

 

If that dosn't work for you use G130. Use Mastercam to create a drilling operation for the holes you want to threadmill. Set macro variables via Manual Entry at start of drilling operation. Edit G83 data and replace with

 

G130R#18Z#26D# etc.

 

The G130 toolpath allows you to choose final arc cleanup or not. I'm not sure if G130 can be used to get a short helix directed inside to outside as you'd probably prefer for threadmilling.

 

Our new machine is KM.

 

I'm going to set up the new machine with tool definitions optimized for EIA. Not even going to turn softjaws with Mazatrol on the new machine till after the EIA definitions are establisted.

[RStuart]

I guess i should have pointed out that I am thread milling a pipe thread. Anyhow, job is done now. Reverted back to simplt tapping it. Also was wondering with the Integrex doesn't compensate for tool diameter on its approaches when doing angled milling. Like when I do a tornado mill at angle it approaches fine but collides with the part on the initial plunge. I always have to do the trig and move my start point. Just seems funny that you tell it so much info and it "knows" so much that it can't do that on its own.

[crazy^millman]

Ok Peter sorry for the mis-understanding. But that was what I mean for the threading operation was all.

 

 

RStuart ask them about the G7 sprial milling they have for the Mazak's if you cant find anything I will go through my book and see if I can find what I have on it.

[McRae]

"There is no such thing as threadmilling in 5 axis mode. "

 

Excellent idea... I would suggest that there isn't anyone that thought of doing this yet, some sort of conical fanning would get the job done, but why?? The form on the threadmill would need to be changed to account for the tilt angle etc...

 

Be neat to see though - especially on the integrex!

[crazy^millman]

Yeah but the tool Clearecne would be a problem the key to doing that. It would not really be that big of a deal to do outside threads with the right tool the inside threads would be the hard part.