messed up threadmill toolpath

[swanny]

I wrote a threadmill program using a 5/8 diameter multi toothed threadmill with 16 threads per inch. I turned off all types of entry and just clicked start at center. So the tool starts in the center at the bottom of the hole, moves perpendicular into the wall and works it way up at my pitch of .0625

 

Well when I post it out, the first quarter of the arc movement it doesn't move in a z axis. Then on the exit, the last quarter of the arc it doesn't move in a z axis. This is giving me overlapping threads. I've never seen this happen before or maybe I just never noticed it. Here is a copy of my post:

 

(THREADMILLS FOR 1-5/8"-16 THREAD)
T6M6(5/8" X 16 PITCH THREADMILL)
M11
G0G90A0.(INDEX)
M10
G5.1Q1
G0G90G54X.0003Y0.S5500M3
G43H6Z6.T4M8
Z5.052
G1Z4.327F50.
G41D6Y-.485F35.
G3X.4853Y0.I0.J.485
X.4853Y0.Z4.3895I-.485J0.
X.0003Y.485I-.485J0.
G1G40Y0.
Z4.327F50.
G41D6Y-.4925F35.
G3X.4928Y0.I0.J.4925
X.4928Y0.Z4.3895I-.4925J0.
X.0003Y.4925I-.4925J0.
G1G40Y0.
Z4.327F50.
G41D6Y-.5F35.
G3X.5003Y0.I0.J.5
X.5003Y0.Z4.3895I-.5J0.
X.0003Y.5I-.5J0.
G1G40Y0.
Z4.327F50.
G41D6Y-.5F35.
G3X.5003Y0.I0.J.5
X.5003Y0.Z4.3895I-.5J0.
X.0003Y.5I-.5J0.
G1G40Y0.
G0Z5.052
Z6.
G5.1Q0
M5
G91G28Z0.M9
G91G28Y0.
G0G90G54X-20.
M201
M30

 

Hopefully someone can figure this out. I know if I turn on helical entry and exit it fixes this. I'm wondering why this would even be an option in a threadmill program. Is this a glitch?

[Myth Project]

Yeah, turn on helical entry.  The only time you might turn off helical entry is when you're using a single point thread mill.  In which case it won't fubar the threads.

 

And the purpose of non-helical entry is to get deeper full threads on a non-through hole, I think.  Had to use non-helical entry one time to get the threads to depth on a part once...  Hopefully this helps in some way.

[swanny]

Still doesn't make sense. I'm already in an arc in the toolpath but it doesn't post a z movement. Its just a basic perpendicular entry. This way I can use cutter comp at the control to size my threads.

[Guest]

Still doesn't make sense. I'm already in an arc in the toolpath but it doesn't post a z movement. Its just a basic perpendicular entry. This way I can use cutter comp at the control to size my threads.

So long as you have a linear move, you'll be able to use/enable comp.

 

The only time I don't have helical entry/exit enabled is when I am using a single point tool; otherwise it's on.

[gcode]

See the attached screen shot

set your lead ins like this

play with the size of clearance arc and watch the lead in /out motion

you want a big arc to get smooth entry motion, but not too big or you won't get a

straight linear move

once you've got a good linear move and good arc motion, you should be good to go

set your comp type to Wear

[swanny]

So long as you have a linear move, you'll be able to use/enable comp.

 

The only time I don't have helical entry/exit enabled is when I am using a single point tool; otherwise it's on.

So its ok to have a quarter of a turn in a thread at the entry without a z movement as long as its single point? Once you are into the thread diameter it should always be moving at the pitch. Single point, multi point, whatever. A quarter of a turn is .015 in this case. So this option is in there so you can use a single point tool in a thru hole and you can start below the thread and want to, for whatever reason, have a quarter of a turn without it moving in the z axis? I get the fact turning on helical entry/ exit eliminates all this, but why have this option at all if the outcome could be a bad thread.

[swanny]

So long as you have a linear move, you'll be able to use/enable comp.

 

The only time I don't have helical entry/exit enabled is when I am using a single point tool; otherwise it's on.

So its ok to have a quarter of a turn in a thread at the entry without a z movement as long as its single point? Once you are into the thread diameter it should always be moving at the pitch. Single point, multi point, whatever. A quarter of a turn is .015 in this case. So this option is in there so you can use a single point tool in a thru hole and you can start below the thread and want to, for whatever reason, have a quarter of a turn without it moving in the z axis? I get the fact turning on helical entry/ exit eliminates all this, but why have this option at all if the outcome could be a bad thread.

[Myth Project]

One part that I programmed recently had a hole depth call out that was too close to the minimum thread depth.  The only way to get enough thread in the hole was to turn off helical entry and cut the thread with a single point thread mill.  Had the option not been there, I wouldn't have been able to produce enough thread.

[Myth Project]

Furthermore, if you had drafted your thread mill and ran a full verification, you should have noticed that it would produce double threads, as I almost made the same mistake once.  I luckily caught mine in verify.  So I say, verify, verify, and verify.  

[swanny]

One part that I programmed recently had a hole depth call out that was too close to the minimum thread depth.  The only way to get enough thread in the hole was to turn off helical entry and cut the thread with a single point thread mill.  Had the option not been there, I wouldn't have been able to produce enough thread.

If you have it turned off then its not threading at the beginning, so what's the difference?

[swanny]

Furthermore, if you had drafted your thread mill and ran a full verification, you should have noticed that it would produce double threads, as I almost made the same mistake once.  I luckily caught mine in verify.  So I say, verify, verify, and verify.  

Who said I didn't catch it?

[Myth Project]

Who said I didn't catch it?

Very true. 

 

If you have it turned off then its not threading at the beginning, so what's the difference?

It did produce usable thread deeper than starting with helical entry would, though you are correct, it did produce some crap thread at the very bottom.  But as long as usable thread was produced to the desired depth, I was covered.  

[swanny]

F.Y.I.-I just got off the phone with an Industrial Division Mastercam tech at CNC Software Inc. This isn't suppose to work like this. He is running more tests on it and will be getting back to me. He ran it on 3 different versions of Mastercam (7,8,9) and was getting the same result.