trouble with thread milling G Code

[BobM3]

I'm trying to make a 3/8-18 internal pipe thread using a 4 flute, .37 Dia. carbide pipe thread mill. I've tried 3 of the online G code generators but I end of having the same problem with each. The programs use tool compensation and I keep getting the same error:

Error 41 "Interference in CRC"

If I set the tool radius small enough (quite a bit less than .185) I can at least get through the code without any error messages.

I believe the problem is in the initial entry arc. Anyone else run into this? I'm sure I'm doing something stupid.

 

[Bobw]

I'm trying to make a 3/8-18 internal pipe thread using a 4 flute, .37 Dia. carbide pipe thread mill. I've tried 3 of the online G code generators but I end of having the same problem with each. The programs use tool compensation and I keep getting the same error:

Error 41 "Interference in CRC"

If I set the tool radius small enough (quite a bit less than .185) I can at least get through the code without any error messages.

I believe the problem is in the initial entry arc. Anyone else run into this? I'm sure I'm doing something stupid.

Post the code.

Is the code using centerline, or full radius/diameter comp.. Is your machine set to use RADIUS or DIAMETER?

$50 says its something stupid that will make you want to smack your head against a vise.
I'm not saying that in a bad way.. Happens to me all the time.

 

[litlerob1]

I'm trying to make a 3/8-18 internal pipe thread using a 4 flute, .37 Dia. carbide pipe thread mill. I've tried 3 of the online G code generators but I end of having the same problem with each. The programs use tool compensation and I keep getting the same error:

Error 41 "Interference in CRC"

If I set the tool radius small enough (quite a bit less than .185) I can at least get through the code without any error messages.

I believe the problem is in the initial entry arc. Anyone else run into this? I'm sure I'm doing something stupid.

I'm being totally pragmatic when I say this, not condescending or just being a dick. BUT we don't even know what type of Machine you are on!! Let alone what control, or version thereof. And without seeing actual code, how on Earth would we help?

We could just start saying things like 42 is the answer, (which has come up several times).

R

 

[Bobw]

I am assuming that is a 3/8 NTP tapered thread. Fun Stuff.
I have had the same problem and ended up just using center line programming. There is not enough room in the hole to apply full cutter comp. If you had a larger thread diameter you would not have the problem.

WAZP

That's BS.. Its all in the programming, simply understanding the lead ins and lead outs... If there is a .0001, there
is enough room, its all in understanding how it works..

Having said that.. I RARELY, if EVER use full R or D comp.. Centerline it is. And honestly I almost never
use any comp at all, unless its a REALLY tight tolerance or something is floppy, and I might have to tweak it in.

Trick to drop in on center when using centerline. Take the differences in RADIUSES, say a 1/2" cutter in a 1" hole.

So .500R - .25R = .25R difference.. Now take that # and multiply by .414.. .1035.. Now in your Cad, lead in line length,
.1035.. Arc, 135 degrees(constant) and a rad of .1035... Drop you right on center every time.

I have it written on the wall above my desk.



Complete nerd diversion. The math on this is simple. Its a triangle and a line. Once you draw it,
you can completely ignore the arc. But the .414 is everywhere. You need the inverse of SIN45, which is
1.414(sqrt2, quadratic will get you there too), then you have to add one, so 2.414, and then the
inverse of 2.414 is .414.. I thought it was kind of interesting.

 

[litlerob1]

Complete nerd diversion. The math on this is simple. Its a triangle and a line. Once you draw it,
you can completely ignore the arc. But the .414 is everywhere. You need the inverse of SIN45, which is
1.414(sqrt2, quadratic will get you there too), then you have to add one, so 2.414, and then the
inverse of 2.414 is .414.. I thought it was kind of interesting.

That is more than interesting, Ive never even tried making a constant value for lead in/out for a Thread. I'm always fucking around with it for a few minutes. Thanks, Bob. I always assumed you were too old to be nerdy

WAZP, I have no idea what you are trying to say; "There is not enough room in the hole to apply full cutter comp". I wouldn't even attempt to Threadmill in the first place if CC was something I couldn't use. If I had to change the G-code every time, I'd freak out. I'd be setting up some crazy Milling part up on a Lathe with a 4 jaw Chuck all the time or something.

R

 

[gkoenig]

$50 says its something stupid that will make you want to smack your head against a vise.

You're using an Orange for that, right?

An old crusty, crummy Kurt falls to pieces when you smack your head against them at a high volume the way I do.

As to the OP? This is a nice opportunity to download Fusion for free and use it to spit out your G code way better than any online calculator will. Saunders even has a decent nerdy video that makes it bulletproof on the first go without having to chase threads (most of the time). How to Threadmill! - NYC CNC

 

[litlerob1]

You're using an Orange for that, right?

An old crusty, crummy Kurt falls to pieces when you smack your head against them at a high volume the way I do.

Dude I wouldn't be spreading your blather across other Threads.

 

[BobM3]

Below is the code from one of the programs. Machine is a Hardinge VMC. Control is a Fanuc0i-MB. The offset screen uses the radius of the tool. I've had trouble using cutter comp on this machine before and ended up just not using it. I'll probably end up doing the same with this.

The error message occurs before the first compensated move:

G41 X0.0648 Y0.0648 D6 F5.53

With look-ahead I'm never quite sure what line is the problem but I'd suspect it's this one combined with the following one or two arcs.

*****************************************************************

NPT/NPTF Thread Mill Single Pass G-Code Program

NOTE!!! ONLY CHANGE THESE VARIABLES TO GET PROGRAM
Major Diameter 0.6292
Cutter Diameter 0.37
Pitch (TPI) 18.0
Full Thd Depth Max 0.407
SFM 250
Feed Per Tooth 0.0013
# of Flutes 4

Threadmill Pitches
Sizes TPI Lead
1/16 & 1/8 NPT 27 0.03704
1/4 & 3/8 NPT 18 0.05556
1/2 & 3/4 NPT 14 0.07143
1" - 2" NPT 11.5 0.08696
2.5-8" NPT 8 0.12500

PROGRAM FOR NPT & NPTF THREADS Internal
Thread description and tool #:
Start point at center of hole in X & Y and top of part in Z
M3 S 2581
G01 G91 Z- 0.41394 F 30.0
G41 X 0.0648 Y 0.0648 D (offset#) F 5.53
G03 X- 0.0648 Y 0.0648 Z 0.00694 i- 0.0648 j 0 F 5.53
G03 X- 0.1300 Y- 0.1296 Z 0.01389 i 0 j- 0.1300 F 5.53
G03 X 0.1300 Y- 0.1305 Z 0.01389 i 0.1305 j 0 F 5.53
G03 X 0.1309 Y 0.1305 Z 0.01389 i 0 j 0.1309 F 5.53
G03 X- 0.1309 Y 0.1313 Z 0.01389 i- 0.1313 j 0 F 5.53
G03 X- 0.0657 Y- 0.0657 Z 0.00694 i 0 j- 0.0657 F 11.06
G00 G40 X 0.0657 Y- 0.0657 F 30.0
G00 Z 0.34450
G90
Note: (offset #) is for the cutter comp. If you are using tool 18, put in D18

NOTE: THIS SHEET IS NOT WRITE PROTECTED. PLEASE SAVE A COPY BEFORE CHANGING.

Diameters for threads with a depth equal to L1+L3
Cutter Major Depth Cutter Major Depth
Thrd. Dia Dia (L1+L3) Thrd. Dia Dia (L1+L3)
1/16 0.237 0.309 0.271 1-1/2 0.595 1.889 0.681
1/8 0.237 0.401 0.273 2" 0.596 2.362 0.697
1/4 0.292 0.533 0.395 2.5 0.713 2.856 0.932
3/8 0.292 0.668 0.407 3 0.718 3.482 1.016
1/2 0.475 0.832 0.534 3.5 0.722 3.983 1.071
3/4 0.477 1.043 0.553 4 0.723 4.481 1.094
1" 0.593 1.305 0.661 5 0.729 5.543 1.187
1-1/4 0.595 1.650 0.681 6 0.731 6.600 1.208
8 0.737 8.594 1.313

 

[Larry Dickman]

I'm being totally pragmatic when I say this, not condescending or just being a dick. BUT we don't even know what type of Machine you are on!! Let alone what control, or version thereof. And without seeing actual code, how on Earth would we help?

We could just start saying things like 42 is the answer, (which has come up several times).

R

The answer is ... 4? - YouTube

 

[Bobw]

The offset screen uses the radius of the tool.

G01 G91 Z- 0.41394 F 30.0
G41 X 0.0648 Y 0.0648 D (offset#) F 5.53

The lead in move is a little over .090" sqrt(.0648^2 + .0648^2).

The program is running centerline/wear comp, and you are putting the full Rad/Dia in
the offset table.. You only need to enter a WEAR value, minus a few thou to go bigger,
plus a few thou to go smaller.

 

[Mtndew]

Complete nerd diversion. The math on this is simple. Its a triangle and a line. Once you draw it,
you can completely ignore the arc. But the .414 is everywhere. You need the inverse of SIN45, which is
1.414(sqrt2, quadratic will get you there too), then you have to add one, so 2.414, and then the
inverse of 2.414 is .414.. I thought it was kind of interesting.

My head just exploded.

 

[litlerob1]

BobM3, I think your offset value is greater than .0324, that is why you are getting an error.

Read Bobw's post #12. See if the program will run with Zero in the offset page, per Radius or Diameter. Leave the G41 alone, but don't use any value at all in the offsets and see if that runs the program without error. I think it will. From there you can start offsetting the Diameter of the Tool. Using Minus values to get a larger diameter.

Plus you should be able to single block it right to the line of code that is giving you errors, if you Single Block it, it won't Alarm on look ahead errors??(maybe).

R

 

[BobM3]

That was is BobW - thanks for the help.