How to ... 5 AX threadmill ?

[HEED]

Hey guys how do I setup to run a threadmill on on a hole that's not normal to the "z" ? I tried some things and I cant get it to work, it always tries to do it in the top plane, when I want it in front.

[crazy^millman]

What toolpath are you using? What C-plane are you using? Are you using a point and lines to drive the toolpath? Can you drill holes using your method with no problem?

[HEED]

I am trying to use the circle mill toolpath in top plane, straight off the toolpath, no point path before, yes I am able to drill the hole no problem just when I go to thread it, it's not quite right...

[crazy^millman]

Got a sample you can share. Save the geometry you are using with save some re-toolpath in that saved file and email it to me or FTP it.

[HEED]

Hi again, I think i may have gotten it figured out,ron. I switched to a different tplane. How, and when do you know when to use different tplanes ? I thought you stayed in top always and used MC to deicde where it needs to move to.

[crazy^millman]

Rule I have is anytime the path does not lay in the top view, and is not a 5 axis toolpath like 5 axis drill, 5 axis curve, ect..... or any of the advanced 5 axis toolpath use must you a c-plane for it to work.

 

Glad you got it figured out.

[HEED]

That makes sense, so can you use a 2d contour on a 5 ax machine, just select the proper tplane ? I have been using 5 ax curve for everything. I guess maybe you would have to use either a 5 ax curve, or 2d and a bunch of point toolpaths, right?

[MIL-TFP-41]

get to know your toolplanes...there are big advantages out there for 2d toolpaths vs 5 ax. Things like cutter comp, much shorter programs (you will actually use G2 or G3 for arcs)

 

So basically in your above example, your WCS should be top & the toolplane & c-plane would be front. Its really easy to do 4 sides of a cube using just your system views/planes...ie front, left, right, back....

[crazy^millman]

quote:

---

That makes sense, so can you use a 2d contour on a 5 ax machine, just select the proper tplane ?

---

That my friend is what they call 3 + 2. Anything you can do 2 or 3 axis can be done this way I mean anything. I use to rough my molds with 3 + 2. I would make my Gview the Cplane then draw my boundary on that cplane and then I knew what my limits where in that plane when cutting my 3 axis toolpaths like surface rough pocket, surface rough parallel. Limits of this are the limits you put on yourself. 99% of the time 2d or 3d contour does the trick in 3+2, but sometimes curve 5 axis is the only thing that will do what you want. I got a machine our Integrex that you can not go from 3 + 2 to full 5 axis without an alarm. Machine issue and Mazak told me tough sh?t they no longer support the Control the Matrix is the one supported so any bugs oh well. Anyway I have make all my 3+2 contour cuts 5 axis once I am in 5 axis. Trying to go back to G68 or any 3+2 work with can be normal 3 axis work give the machine and alarm and I have to call a tool change so the operator can reset and start from there. Sucks, but the way I have to program on this $%#%@#$$% machine.

[HEED]

That's some good information, right in the last 2 posts, thanks james and ron I have been using 5 ax curve for EVERYTHING and it's not only a pain in the @$$ to program, but the feed rates are wierd, ( entry / exit and retract are now feedrates? ) I am happy to find out you can use 2d curves and paths in 5 ax machining. I have been using strictly 3+2 so far with no simul 5 ax moves, so this is big for me thanks guys ! Another question that may be off topic, but why do machine tool manufacturers ALWAYS cut an impeller as a demo on a 5 ax machine ? It seems that 75% or more of 5 ax machining is 3+2. I dont know much about blisks, impellers, etc. are they just incredibly complex with angles, etc.?

[crazy^millman]

To the majority Yes to people who know 5 axis really well no. They can be tricky I have seen some really out their designs, but once you do a couple of them they are just another part. Biggest thing Is really thinking about what effect one has to the next one. Some people like to cut every other, some like to skip around and some like to cut one right next to the next one just depends on the material, the thickness of the vanes, complexity of the vanes, and if it gets heat treated all play important parts of making one correct.