lots of problems

[EHA]

I'm trying to do a npt thread mill op.... I can't get it to output cutter comp, I've tried generating code with the controller and pathrace selected for the comp. Why is it doing this? The other thing is when I do a canned cycle so it will give me a g3 line instead of point to point it says errors in program right before the code editor window comes up, then in the program its tellin me that the threads may be innacurate. I have no idea, I've tried changing the output tolerance from .001 all the way down to .00001. Still does it. Any ideas?

[inflateable]

Can you post the output with the errors in? Might be able to pick up a clue from that.
I'm guessing that it might be warning you that your controller might not support 3D G3 moves (i.e. moving in X,Y and Z simulataneously in a helix)

[Mike Mattera]

I doubt if your machine does comp on a helical move. I would see if the control supports it before you worry about the output of the post.

Mike Mattera

[Mike Stevenson]

Originally Posted by Mike Mattera I doubt if your machine does comp on a helical move. I would see if the control supports it before you worry about the output of the post. Mike Mattera

Actually most Hass, Fadal, and Fanuc controls will do G41 XY comp on helical moves with the Z being a linear move without comp.

[rayzer]

The threadmilling cycle within edgecam always gives me headaches.

the cycle is very old does not work correct with radius compensation, and whem simulating the toolpath in edgecam machine simulator the tool offsets are wrong and result in maximum overcutting.

radius compensation turned on with a conical rampdown has never worked for me with this cycle in edgecam, so i program that from hand just like every Edgecam user i know.

Good luck.

[helix77]

i use it all the time.... i usualy have to adjust the thead info (thread tab) to fine tune .... or i can use the old left compensation icon before the cycle.... i can get it to post a g41 on the lead in...but no matter what i do it will not post a g40 on the lead out....i just hand code it in in editer somewhere above the part
this cycle definatly needs to be re-thought

[timf]

comp on thread mill was one of the updates for 12.5.
you have to update your genrator file and check the option but i think it works no with the new thread mill box.
i haven't tried a tapered thread but i got a regular one to kick out with arcs and comp.
i'm still going to tweak a little for my own comfort to see code in the order i want but it was close enough to use i thought at the time.
i have to go back and check it out more.
even my older fadal will acknowlegde comp on helical moves even though i thought for years they wouldn't till i had an operator tell me he put it in the program and it worked.

[invs879]

I can get one 360º pass with lead in/out generated for an NPT. It took me about an hour of reading the help files for thread milling. Helpless help.

I want to use a single point thread mill and generate 8 continuous 360º passes following the NPT taper. I do not think edgecam provides this solution.

Probably must create 8 processes at adjusted Z and Radius and then work on lead in/out.

Lots of fun.

[inflateable]

The help files in Edgecam are almost worthless - I had some edgecam training a few weeks ago and even the trainer was baffled by some of the 'help'.

Anyway, if you're fed up with trying to get edgecam to do something it's supposed to do, if you go to the Seco tools website they have a threadmill wizard you can download. Fill in the details of your thread and it'll output the code to threadmill it. It's meant for seco tools, obviously, but you can use it for any type of tool and it supports comp.

[invs879]

I found micro100.com to provide the most flexible npt thread milling code generator. Its in a spread sheet and does not default to a vendor selection of predefined tools.

This last sunday I browsed Melintools.com, seco.com and micro100. I used Google, groups, alt.machine.cnc " npt thread mill" to search.

Vardex, Kennametal, and Advent all use the same thread mill program tied to one of their products.

No where did I find the single point thread mill program I was looking for. Perhaps I need to search lathe thread mill for npt.

[inflateable]

I have a a parametric thread mill program if you'd like to try that out.

I think if you want to single point it you just need to edit the code a thread mill generator will output. Most of them arc on, arc around to 180deg moving half the pitch in Z, arc around back to 360 completing the pitch in z, and then arc off, If you take the arc to 180, and the arc to 360 moves and copy and paste them, editing the z positions, you can do as many threads as you like.

so if your basic thread mill prog looks something along these lines:
N30 Z-17.0
N40 G03 X0 Y8.5 R6.25
N50 G03 X0 Y-8.5 Z-16 R8.5
N60 G03 X0 Y8.5 Z-15 R8.5
N70 G03 X0 Y-4 R6.25

You'd edit it to something like this:
N30 Z-17.0
N40 G03 X0 Y8.5 R6.25
N50 G03 X0 Y-8.5 Z-16 R8.5
N60 G03 X0 Y8.5 Z-15 R8.5
N50 G03 X0 Y-8.5 Z-14 R8.5
N60 G03 X0 Y8.5 Z-13 R8.5
N50 G03 X0 Y-8.5 Z-12 R8.5
N60 G03 X0 Y8.5 Z-11 R8.5
N50 G03 X0 Y-8.5 Z-10 R8.5
N60 G03 X0 Y8.5 Z-9R8.5
N70 G03 X0 Y-4 R6.25

Obviously I'm just making these numbers up, but that should give you the gist of it.




Y

[helix77]

THIS IS THE BLOCK OF CODE I USE AFTER THE POSITIONING MOVE TO GET THE THREADMILL WHERE IT NEEDS TO BE...

G91 G03 X? Y? I? J? Z? L?
G90
WHERE THE L IS FOR LOOP FOLLOWED BY THE NUMBER OF TIMES TO REPEAT THE HELIX
THIS IS FOR THE HAAS I USE... THIS IS ALL I EVER USED BEFORE I FIGURED OUT THE THREAD MILLING CYCLE..

YOU CAN ACTUALLY USE THE PROFILING CYCLE WITH HELICAL CHECKED AND CUTTING CONVENTONAL INSTEAD OF CLIMB... (FOR RIGHT HANDED THREAD)... WHERE THE CUT INCREMENT IS THE PITCH