[Geof]

The thread milling code does work fine. The code for the Woodruff cutter was wonky as I explained above.

[brianp-jag]

the code for the wood cutter might look wonky but really does work. seriously it does have made several test cuts and it works. its somethin with the threadmill tho. not sure what tho. anyways im not sure what to do anymore bought to lose my mind. cant get gibbs to do it right or advent. been trying everything you guys have told me to do with no success

[dcoupar]

I may be missing something here, but it looks to me like the woodruff key cutter is absloute I,J and the thread mill output is incremental I,J (distance from start to center).

I don't see a setting in the Advent UI for obtaining absolute center coordinates.

Snippet from your original code:

N435T7M6
/.375 KEY CUTTER
/THREAD RELIEF
/.375X.0625WOODRUFF
N261G0G17G70G90S360
N262G75M3
N263X0.Y0.
N264Z1.
N265Z.1 M8
N266G1Z-.33F.7
N267G41X.1275
N268G3G17X0.Y.1275I0.J0. <-------- Absolute arc center location???
N269G17X-.1275Y0.I0.J0.
N270G17X0.Y-.1275I0.J0.
N271G17X.1275Y0.I0.J0.
N272G40G1X0.
N273G0Z.1
N274M9
N275M25
N276M5
N277 T8M6
N278 M0
/ OPERATION 10: HOLES
/ WORKGROUP
/ ADVENT 5-8--11 THREADMILL
N436 G00 X0.0000 Y0.0000
N437 Z1.0
N438 Z.1 M8
N439 S1543 M3
N440 Z-0.2845
N441 G1 X0.0014 Y-0.0047
N442 G41 D28 X0.0072 Y-0.0238 F4.9
N443 G3 X0.0470 Y0.0000 Z-0.2700 I0.0128 J0.0238 F0.5
N444 Z-0.2144 I-0.0470 J-0.0000 F0.8 <---- Incremental arc center???
N445 X0.0072 Y0.0238 Z-0.1999 I-0.0270 J-0.0000 F0.5
N446 G1 G40 X0.0000 Y0.0000 F40.0
N447 G0 Z-0.2863
N448 G1 X0.0006 Y-0.0049
N449 G41 D28 X0.0031 Y-0.0247 F4.9
N450 G3 X0.0560 Y0.0000 Z-0.2700 I0.0207 J0.0247 F0.6
N451 Z-0.2144 I-0.0560 J-0.0000 F0.9
N452 X0.0031 Y0.0247 Z-0.1982 I-0.0322 J-0.0000 F0.6
N453 G1 G40 X0.0000 Y0.0000 F40.0
N454 G0 Z-0.2871
N455 G1 X0.0003 Y-0.0049
N456 G41 D28 X0.0015 Y-0.0249 F4.9
N457 G3 X0.0620 Y0.0000 Z-0.2700 I0.0251 J0.0249 F0.6
N458 Z-0.2144 I-0.0620 J-0.0000 F1.0
N459 X0.0015 Y0.0249 Z-0.1974 I-0.0354 J-0.0000 F0.6
N460 G1 G40 X0.0000 Y0.0000 F40.0
N461 G0 Z-0.2874
N462 G1 X0.0001 Y-0.0049
N463 G41 D28 X0.0007 Y-0.0249 F4.9
N464 G3 X0.0650 Y0.0000 Z-0.2700 I0.0273 J0.0249 F0.6
N465 Z-0.2144 I-0.0650 J-0.0000 F1.0
N466 X0.0007 Y0.0249 Z-0.1970 I-0.0370 J-0.0000 F0.6
N467 G1 G40 X0.0000 Y0.0000 F40.0
N468 G0 Z0.0100 M5
N469M9
N470M25
N471G90G0M5
N472M2
E

[Geof]

I may be missing something here, but it looks to me like the woodruff key cutter is absloute I,J and the thread mill output is incremental I,J (distance from start to center).....

I forgot some machines interpret I and J as absolute location.

Editing the Advent code would be possible but a bit tedious.

[texaspyro]

The Hurco, in BNC (Basic NC) mode has abs arc centers in G90 mode and incremental arc centers in G91 mode. This is also how most other machines that support absolute arc centers work. Mach3 has a G90.1/G91.1 command for selecting the arc center mode (and be careful using it since it also sets the mode in the System Config file!!!).

A couple of glaring errors: after line N212 is a bad line (GO ...) not G0 and at line N372 is a number with 2 decimal points.

Also, you probably should not be using the '/' block skip command for comments. Many machines will attempt to parse the gcode after the '/' even though it will not be executed. Hurco's should accept (Comment Text) comments.

[texaspyro]

Attached is a preliminary 3d DXF file of the tool paths. The bad line mentioned above was commented out and the extra decimal point removed.

Not sure, but it looks like tool 7 is not doing what you expected.

Also, my DXF converter converts helical arcs into lots of small lines since DXF does not actually support helixes (despite what the DXF2012 spec says). There is a small problem with either your gcode input helix or my dxf output helix end points (but it works with a every other test case I gave it).

If you don't have a 3D DXF viewer, try CAFF.DE for a really nice free one. If you don't have JAVA, you will need to download it from JAVA.COM

[brianp-jag]

thanks for the replies but i have the problem fixed. the problem was in the advent software that came highly recommended. i fixed it with gibbs. everything works good and no longer have the issue. although i will never use the advent stuff again. was told it was easier to use. now that i have it figured out in gibbs thats way easier and works better. also the block skip mode has nothin to do with the problem and the woodruff cutter section was programed by a friend. it looks wierd but works fine on the machine.wrks perfect acctually. thanks for the input though. all is fixed in my world for now.

[texaspyro]

I did figure out why my DXF output routine was messing up on the helical cut endpoints. It turns out that those helical cuts don't have a proper center point specified... it's the old "RADIUS TO START OF ARC DOES NOT MATCH THE RADIUS TO END OF ARC" error that everyone is probably all too familiar with.

Mach3 usually complains loudly about such things, but was happily accepting the Mach3 compatible NC code that I generated from the Hurco input and showed a reasonable looking tool path display. I tweaked my DXF converter so that it slews the radius value between the start and end point radii as it breaks up the helical cuts into multiple small linear pieces. The results match what Mach3 was showing.

[RalphWilson]

Since the starter of this thread is satsfied that he has a answer.
I'd like to start something new, but the same issue.

I am using a fanic controler, ie. A Fadal 15. 10k spindle and no "C" ,or ability to know where the spindle is, NO G84 .
Ok I made the tool path in mastercam x5 , to do a pipe thread. with a thread mill.
I did a ramp in from the center down about 4 threads and around down one thread, and out back to center with a ramp down 1/4 thread.

I did not like the depth of the thread so I droped the hight offset down three threads and adjusted the D offset out to .343dia. G41/G42 at what ever mastecam spit out.
I was happy with the out come and just ran My first ever thread mill.
Now I was lost at the beginning, and confused in the middle, and worryed the next day.
I just ran twenty junk parts or what?

Here is my issue.

THE Thread mill is tapered and the pipe thread is tapered.
I started one thread up and went one thread down.
AS IF the threads were straight , and not tapered.
So I got a flat on one side of the threads and a full thread on the other side.

How can I calculate the true path to make a complete thread all the way around with a tapered thread mill.

This is some what what I did.
(.343 DIA. 18 TPI THREADMILL)
G00 G43 H4 X0.000 Y0.000 Z.100
G01 G90 X0.000 Y0.000 Z0 F50.
(SET D TO AMOUNT OF FIRST CUT)
#D4=.025
S3000 F10.
G42 D4 G02 X0.127 Y0.000 Z-.028 I0.063 J-0.000 K0.000
G02 X-0.127 Y0.000 Z-.083 I-0.127 J0.000 K-0.028
G02 X0.127 Y0.000 Z-.166 I0.127 J-0.000 K-0.028
G02 X-0.127 Y0.000 Z-.249 I-0.127 J0.000 K-0.028
G02 X0.126 Y-0.011 Z-.277 I0.126 J-0.011 K0.000
G40 G02 X0.000 Y-0.000 Z-.305 I-0.063 J0.006 K0.000
G41 D4 G03 X0.127 Y0.000 Z-.277 I0.063 J-0.000 K0.000
G03 X-0.127 Y0.000 Z-.249 I-0.127 J0.000 K-0.028
G03 X0.127 Y0.000 Z-.166 I0.127 J-0.000 K-0.028
G03 X-0.127 Y0.000 Z-.083 I-0.127 J0.000 K-0.028
G03 X0.126 Y-0.011 Z-.028 I0.126 J-0.011 K0.000
G40 G03 X0.000 Y-0.000 Z0 I-0.063 J0.006 K0.000

[angelw]

Since the starter of this thread is satsfied that he has a answer.
I'd like to start something new, but the same issue.

I am using a fanic controler, ie. A Fadal 15. 10k spindle and no "C" ,or ability to know where the spindle is, NO G84 .
Ok I made the tool path in mastercam x5 , to do a pipe thread. with a thread mill.
I did a ramp in from the center down about 4 threads and around down one thread, and out back to center with a ramp down 1/4 thread.

I did not like the depth of the thread so I droped the hight offset down three threads and adjusted the D offset out to .343dia. G41/G42 at what ever mastecam spit out.
I was happy with the out come and just ran My first ever thread mill.
Now I was lost at the beginning, and confused in the middle, and worryed the next day.
I just ran twenty junk parts or what?

Here is my issue.

THE Thread mill is tapered and the pipe thread is tapered.
I started one thread up and went one thread down.
AS IF the threads were straight , and not tapered.
So I got a flat on one side of the threads and a full thread on the other side.

How can I calculate the true path to make a complete thread all the way around with a tapered thread mill.

This is some what what I did.
(.343 DIA. 18 TPI THREADMILL)
G00 G43 H4 X0.000 Y0.000 Z.100
G01 G90 X0.000 Y0.000 Z0 F50.
(SET D TO AMOUNT OF FIRST CUT)
#D4=.025
S3000 F10.
G42 D4 G02 X0.127 Y0.000 Z-.028 I0.063 J-0.000 K0.000
G02 X-0.127 Y0.000 Z-.083 I-0.127 J0.000 K-0.028 - 0.055
G02 X0.127 Y0.000 Z-.166 I0.127 J-0.000 K-0.028 - 0.083
G02 X-0.127 Y0.000 Z-.249 I-0.127 J0.000 K-0.028 - 0.083
G02 X0.126 Y-0.011 Z-.277 I0.126 J-0.011 K0.000
G40 G02 X0.000 Y-0.000 Z-.305 I-0.063 J0.006 K0.000
G41 D4 G03 X0.127 Y0.000 Z-.277 I0.063 J-0.000 K0.000
G03 X-0.127 Y0.000 Z-.249 I-0.127 J0.000 K-0.028
G03 X0.127 Y0.000 Z-.166 I0.127 J-0.000 K-0.028
G03 X-0.127 Y0.000 Z-.083 I-0.127 J0.000 K-0.028
G03 X0.126 Y-0.011 Z-.028 I0.126 J-0.011 K0.000
G40 G03 X0.000 Y-0.000 Z0 I-0.063 J0.006 K0.000

The attached picture is a Plan View back plot of your tool path. It, and a quick look at your code indicates that there are errors in your program. Without going any further, the first line of the tool path, shown in red above, has an incorrect I value for the X end point being programmed.



1. None of the K values are required if a Z end point is specified in the way your code is written. In your example, I believe there would be a conflict as the K value is specifying the correct height move of half of 18TPI, but the Z has specified a greater move. You don't mention the model of the controller, but it would have to have Conical Interpolation to use I,J,and K. Q can also be used to specify the Radius increment or decrement per spiral revolution if Conical Interpolation is available.
2. Post the model of the control and if it has Conical Interpolation available. If you have this function, and it would appear that you may, the thread can be programmed by specifying the Z end point of the thread, K to specify the height increment, and Q to specify the radius increase or decrease.
3. It appears that the code is winding down to the bottom of the thread and then winding out. I would start at the bottom of the thread and wind out so that the tool is climb milling and if you want to take a finishing cut, take the tool to the bottom of the hole and repeat.
4. Don't alter the finish point of the thread by dropping the height offset down. If you mean you changed the Z work shift, this will affect all other tools in the program. If you mean that you changed the tool length offset, this may have disastrous results if this tool is used in other programs and the tool length has not been corrected. If you want the finish point of the thread to be deeper, change the program, not offsets.
5. You state that the thread mill is 18 TPI. That would equate to an axial move of 0.0556 per 360deg rotation around the tool path, ie., from X0.127 to X0,127. In your program example, each circular interpolation block is only 180deg. Accordingly, the Z move should be half the thread lead, or 0.0278, yet the first circular interpolation after the tool is engaged with the work is 0.055, then 0.083 and 0.083 and so on. See the data highlighted in Blue above.

Regards,

Bill

[brianp-jag]

i agree with anglew. i would reprogram to start at the bottom and thread mill up. climb cutting is better. start at your bottom z depth of the thread. DO NOT use your offsets or work shift to change the depth. as angle said you will end up with very bad results and possibly crash the machine or tool. also by shifting your offsets like you did is the reason you have flat spots inside your thread. you should never try and move up or down in your offsets to compensate for a bad program in your thread.

[RalphWilson]

Sorry the code I used before was "SOME WHAT", of what I did.

This is exactly what I did.
This is the code I used. Without modification. this is what I posted to the machine. right out of mastercam.
Notice that there is no "K's in it , but it's going from the top to the bottom then back up and back down then back out.

The post I submitted was out of CIMCO edit, With the K's".
Sorry I was to lazy to re-wright the program in staid of just dropping the "H" value and running the Z to down two threads.

And before you preach about setting the height offset set is a bad habit and all of that.
Wow been there.

I told mastercam that I wanted to start at the top and yes... Oh Boy... Conventional mill the threads ...
I did not know there was a option to mill pipe threads in master cam... until today. My Bad.
I've been a machinist for over 30 years, this is my first opportunity to program a thread mill. Let alone a pipe thread.

(........more code above........)
(................)
T16 M6 (  3/8 X 18TPI THREAD MILL  TOOL - 16  DIA. OFF. - 16  LEN. - 16  DIA - .375 )
G0 G90 S6000 M3 E1 X0. Y0.
H16 Z.25
Z.1
G1 Z-.4167 F0.
G42 D16 Y.2225 F10.
G2 X.3225 Y0. Z-.4306 I.0845 J-.2225
X-.3225 Y0. Z-.4583 I-.3225 J0.
X.3225 Y0. Z-.4861 I.3225 J0.
X0. Y-.2225 Z-.5 I-.238 J0.
G1 G40 Y0.
Z-.4167 F0.
G42 D16 Y.225 F10.
G2 X.325 Y0. Z-.4306 I.0846 J-.225
X-.325 Y0. Z-.4583 I-.325 J0.
X.325 Y0. Z-.4861 I.325 J0.
X0. Y-.225 Z-.5 I-.2404 J0.
G1 G40 Y0.
G0 Z.1
Z.25
M5
G90 H0 Z0.
E0 X0 Y0
M30
(........more code below........)
(................)

I only did this to machine the thread.

When I was home. I drew the other code because I wanted to fix the issue. of the hight offset set .166 below the top of the part, and elemilate 3 inches of rappied moves , by starting at the top and not the bottom of the thread , just like you would tap the thread.

So are we straight on the issues?

I'm sorry.

brianp-jag i agree with anglew. i would reprogram to start at the bottom and thread mill up. climb cutting is better. start at your bottom z depth of the thread. DO NOT use your offsets or work shift to change the depth. as angle said you will end up with very bad results and possibly crash the machine or tool. also by shifting your offsets like you did is the reason you have flat spots inside your thread. you should never try and move up or down in your offsets to compensate for a bad program in your thread.

I am the only person that programs or operates this machine. I included in the program a note to myself the fact that I dropped the height offset by .166, and the next opp the tool will be reset back to the top of three fixture offsets as well.
I just took a short cut. I knew the risks.

No punn intended. Thanks.

Ok since I did not run the first code, only in the simulator. and you included a nice drawing , please redo the drawing with the real code.

Turn it side ways, And draw a circle at the top at the theoretician dia of the top of the pipe thread and then make a cone cut downward to the small end of the thread . using a .75" x 12" ratio , or .75"TPF .
Please notice that the code does not compensate for the increase of 2 times the taper on one side and makes the flat thread.
.................................................. ...................
A web site has the cutter at .310dia at the bottom.
I'm sorry I left my machinist hand book at work, so Excuse me if I have the wrong value for the size of the thread.

At the machine I had a plug Gage and just bumped the "D offset to .343 to achieve the size of the thread. to the flat ground on the plug Gage. and by dropping the starting depth by 3 threads I got just a deeper threaded hole.


I did not notice the flat on the threads until I ran a bunch of them.

SO BACK TO What I asked before : """"" Is there a way to code it with the concoction for the angle ?"""""
I will reprogram it in Mastercam tomorrow to use the pipe thread , instead of just a thread ; as I did , and see if there is any changes in the code.

[Geof]

......SO BACK TO What I asked before : """"" Is there a way to code it with the concoction for the angle ?""""".....

The concoction is to spiral out or in depending whether you are going up or down so your tool follows the taper. I have seen code that approximates this using lots of arcs. I guess this is how mastercam will handle it.

[brianp-jag]

if you have a tapered thread mill for your tapered thread you only need to make your hole to the minor size on the small side of the taper. the thread mill will do the rest for you. you dont need to cut the taper in it. but yes you should also program it for the tapered thread and not for the straight thread. ive only been programming this stuff for a short time myself. i know it can get confusing and frustrating as i only made my first thread mill a couple of weeks ago. i use gibbscam tho. it shouldnt be much different. but you should start at the bottom and climb cut up. the threads come out nicer. also you can take it all in 1 pass and be done. the taper will be there and use your diamiter offset to get your size. it will do it and it looks nice. any more problems repost and i will help best i can. they helped me alot on here but mostly figured it out on my own with the help files in gibbs. surely mastercam has them also. i suggest you read them if you have them. they are a major help.

[RalphWilson]

Thanks for your help, I guess I am just stuck on conventional milling. and was afraid of doing it wrong and assuming the thread mill would somehow pull the part out of the vice. by going from the bottom up climb milling.
I was sufing around and found a downloadable program at

www Vardex com
Software For Thread Milling Tool Selection and CNC Programming
New Version

Vargus' TM Gen, a PC-based program, guides you through a few simple steps to define the thread milling application and then providing all the information needed to complete your threading job - the best threading tool to use, the optimal machining data, and the actual G-code for all popular controllers
http://www.vargus.com/download/files....0.5-Light.exe

I did the steps and spit out this from the program

%
O0001(TMINRH CLIMB INCH CYCLES =1)
(Tool cutting diameter = 0.305 inch - Fanuc 11M Controller.)
(Taper=1/32.0 dAlfa=22.5  Second Loop Teeth=0)
G90 G00 G57 X0. Y0.
G43 H1 Z2. M3 S9968
Z-0.4137
G01 G41 D1 X0.1017 Y-0.2334 F13.04
G03 X0.3351 Y0Z-0.4078I0J0.2334 F13.04
G03 X0.2371 Y0.2371 Z-0.4009 I-0.3352 J0.0003 F43.47
G03 X0.0000 Y0.3355 Z-0.3939 I-0.2373 J-0.2370
G03 X-0.2374 Y0.2374 Z-0.3870 I-0.0003 J-0.3356
G03 X-0.3359 Y0.0000 Z-0.3800 I0.2373 J-0.2376
G03 X-0.2377 Y-0.2377 Z-0.3731 I0.3360 J-0.0003
G03 X0.0000 Y-0.3364 Z-0.3661 I0.2379 J0.2376
G03 X0.2380 Y-0.2380 Z-0.3592 I0.0003 J0.3365
G03 X0.3368 Y0.0000 Z-0.3522 I-0.2379 J0.2383
G03 X0.1034 Y0.2334 Z-0.3463 I-0.2334 J0
G00 G40 X0. Y0.
Z-0.4143
G01 G41 D1 X0.0994 Y-0.2421 F13.04
G03 X0.3416 Y0Z-0.4078I0J0.2421 F13.04
G03 X0.2417 Y0.2417 Z-0.4009 I-0.3417 J0.0003 F43.47
G03 X0.0000 Y0.3420 Z-0.3939 I-0.2419 J-0.2416
G03 X-0.2420 Y0.2420 Z-0.3870 I-0.0003 J-0.3421
G03 X-0.3424 Y0.0000 Z-0.3800 I0.2419 J-0.2422
G03 X-0.2423 Y-0.2423 Z-0.3731 I0.3425 J-0.0003
G03 X0.0000 Y-0.3429 Z-0.3661 I0.2425 J0.2422
G03 X0.2426 Y-0.2426 Z-0.3592 I0.0003 J0.3430
G03 X0.3433 Y0.0000 Z-0.3522 I-0.2425 J0.2428
G03 X0.1012 Y0.2421 Z-0.3458 I-0.2421 J0
G00 G40 X0. Y0.
G90 G00 Z8.0000
M5
M30
%

I maxed the speed of 10000RPM's to do the thread in 6 sec.
Wow that's fast.

I can't tell by looking at the code to see if it addresses the fact that the taper is on the side of the cutter as well as the taper is on the part being machined to make the thread "round or conical in shape. I think the only way to make it round is to follow the real geometry in a segmented action like

.......I have seen code that approximates this using lots of arcs. I guess this is how mastercam will handle it......

he suggested.

or I mite just have master cam draw a Spiro in a cone and transpose into a smaller Spiro; resembling the center line of the cutter and create a contour of 4 or five thread pitches at the angle of the taper.

This should give me comfort in knowing the thread would be round, and the error for a flat thread would be gone.
The only thing that bugs me is that , Yes I could mill the thread in one pass.
And yes conventional mill it in more aggressively than climb milling the thread.

I'll make one cylinder the size of the drilled hole and one cone the size of the finished cone resembling the outside cone of the thread and still another of the cone resembling the finished inside diam or the material at inside sticking in.
My first pass into the threads will cut the crest of the thread and plunge into the bottom or root of the thread, almost like you would on a lathe then flow around one pitch down and one more time around to pick up the out of roundness.

Then

Pull all my hare out.
well maybe,




I still going to do it in mastercam.

[Geof]

That is the code, or very similar.

See the dAlfa=22.5 near the top, that is the angular distance of the arc. When I single block it through graphics on my Haas you can see the individual arcs.

[RalphWilson]

That is the code, or very similar.

See the dAlfa=22.5 near the top, that is the angular distance of the arc. When I single block it through graphics on my Haas you can see the individual arcs.

I wonder if My fadal will understand that code.
I will see if it allows it.
I'm going over to the parabolic programing section of CNC zone site, so as not to change the subject here.
I'm making a thread milling micro, so I don't have to work so hard next time.

Thanks.

[angelw]

I wonder if My fadal will understand that code.
I will see if it allows it.
I'm going over to the parabolic programing section of CNC zone site, so as not to change the subject here.
I'm making a thread milling micro, so I don't have to work so hard next time.

Thanks.

As suggested in my first post, let the Forum know the model Fanuc control your machine has. If your control has Conical Interpolation, you will be able to program the tapered thread in one block.

Whether you use a tapered milling cutter, and the thread is machined in one helical rotation, you still have to accommodate the change in radius during the one thread lead the Z axis will travel.

Regards,

Bill

[brianp-jag]

you can also go to advent thread milling and use there downloadable softeware to. it gives you all the info you need and you just plug in some numbers and it does it. it has options for tapered and straight threads. i had good luck with the tapered threads not so much with the straight threads. also they have several choices for posts.