Showing results for 
Search instead for 
Do you mean 
Reply

Tapered Threadmilling

Anybody know how to single point threadmill an I.D. thread with a 10 degree taper? I'm looking for circular output every 45 degrees.
15 REPLIES

Re: Tapered Threadmilling

Technically, the curve described is NOT a G2/G3 helix that any control I know of can follow (radius constantly changes with "Z" axis, assuming Z axis is along CL).  Yes, people approx. pipe threads with helices, but (to me) thats ugly.

 

As this *looks like* a pipe thread (i.e. same problem, but different values), I would create a law curve spline at the proper tool CL and drive the tool along it.  Yes, you get 100s of G1 moves, but such is life.  (I created a deformable part to do pipe threads - so tool dia, etc. can be easily modified)

 

If that is not to your liking...

I would create the helix curves as geometry and then drive along them.  That way the geometry can control the tolerancing.

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Tapered Threadmilling

Hi Ken, Yes, I'm cheating and you're onto me! Actually It was the first time I had seen it done that way but the existing output (done manually) is G03's with the Z value changing by 1/8 of the lead every 45 degrees. It also is using cutter comp and that works good too. Like you said, it's not really an arc but I guess it's close enough every 45 degrees that it works. I divided the spline into 45 degree segments and ran a planar mill op on it and got my G03 with X,Y,I AND J values all good but now I'm manually adding in Z depths. I'd love for the threadmilling module to take care of tapered threads!

Re: Tapered Threadmilling

I've seen it somewhere else too (maybe thread mill tool manufacturer?) - implemented as a macro (one for each thread size - yecch!)

 

What I did to make it easier for straight threads, could be applied to your case

- Create a UDE to specify the pitch

- handle UDE during arc moves

(recalculate Z=mom_pos(2),  mom_last_pos and mom_prev_pos, also maybe mom_pos_arc_center) - you may have to play a bit to get it to behave well.

- I just ignore it during linear moves

 

Or something like that.

There is a variable to determine how much included angle the arc has so you can appropriately calculate the Z delta (mom_arc_angle).

 

But I'd still go the "create the geometry" route and use FASC to machine it.

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Tapered Threadmilling

Thank you for help, Ken. As always, I appreciate it.

Re: Tapered Threadmilling

[ Edited ]

 

Some machines have spiral/tapered helix interpolation 
G2.1 & G3.1
G3.1X Y Z I J P
X Y are end point coordinates (end radius)
I J are start radius (incremental from start point)
P number of pitches (Revolutions)

 

It would require a UDE or custom cycle to get full output from UG

I have output simple planar mill / hole-milling operations and use notepad++ regular expressions to get usable code.

 

Alternatively for older machines I wrote a macro in macro-B and use a drill text cycle for inputs

 

Here is a very simple example without checking, OD or starting from the bottom.

 

More segments equals smoother thread, however some of the older controls choke if you get carried away

 

(TAPERED HELIX MACRO)
(G65 P9030 A C D E F K R S X Y Z)
(A=#1=SIDE ANGLE) (C=#3=DIR 1=ANTICLOCKWISE -1=CLOCKWISE) (D=#7=START DIA) (F=#9=CUT FEED) (K=#6=PITCH) (R=#18=START HEIGHT Z) (S=#19=SEGMENTS) (X=#24=CENTRE X) (Y=#25=CENTRE Y) (Z=#26=END Z) #33=#5003(SAVE Z) #30=0(CURRENT ANGLE) #31=#18-#26(Z TOTAL) #32=0(CURRENT Z INC) G090X#24Y#25 Z#18 G1X[#24+#7/2]F#9 WHILE[#32LT#31]DO1 #30=#30+360/#19 #32=#6*#30/360 #29=#7/2-#32*TAN[#1](CURRENT RAD) G1X[#24+#29*COS[#30]]Y[#25+#3*#29*SIN[#30]]Z[#18-#32] END1 X#24Y#25 G0Z#33 M99

 

 

Re: Tapered Threadmilling

Very nice! Thank you Agrivas!

Re: Tapered Threadmilling

NXCAM delivers a solution for NPT thread where the output consists of approximating helicals, but NXCAM doesn't (yet) support custom taper angles. You may contact GTAC to register an ER if needed.

 

 

Thanks,

 

Toon

Re: Tapered Threadmilling

[ Edited ]

Why doesn't Siemens get on board with today's technology?

We've been milling tapered threads for about 10 years in medical industry.

Not to mention that some are even double and triple lead.

 

One of our users convinced our management to purchase one seat of SolidCAM because he was getting frustrated with all the things NX cannot do for about 1/5th of what NX costs.

He punched in whatever thread taper I wanted, whatever pitch, and he got a nice simple output with G03 moves.

 

NX can't even recognize a tapered hole in the new Hole Milling Operation!

 

Meanwhile Siemens needs to collect Enhancement Requests to implement something that simple?!?!?  Really? Send your software developers into today's manufacturing shops.  Have them look at all the cutters, threadmills, and various tools your software cannot handle.  Tell them to start moving...  others are way ahead of you for fracture of the cost.

 

Meanwhile I'm writing my code in excell spreadsheets... over 16 years of NX experience.

 

Jerry

NX8.5

Re: Tapered Threadmilling

You're right Jerry. There are thousands of dental and othopedic parts with 20 degree tapered threads in them. Why limit the tapered thread to 1 NPT style. If the function is in NX for 1.79 degrees why can't it be available for other angles.

Learn online





Solution Information