Making a multi-index interrupted thread in mastercam 2020 Mill Turn

[AGreen5]

I found Mastercam 2020 thread milling in Mill-turn to be a little lacking as it pertained to multi-index threads.   This post details the closest thing to a solution I was able to find.  

I had a part I designed that I needed a multiple index thread on.  Thread milling allows the start angle call out, and linking parameters allows a a very small value like .018" to be the top of stock to depth, but the program outputs a full 360 helix disregarding the linking parameters which are calling for ~18% of a helix.  

So I tried to cut a spline in 3D contour lieing and saying the tool was an end mill with the major diameter of the thread mill  (a single linear arc with different Z start and end) and it output that in dozens of linear moves (not one single arc move).  That was a very hard geometry to draw as far as I know in mastercam, I made the line using  3D curve on edge from a solid model.  I called Shopware and they messed with arc filter settings to get smaller facets (more points).  This improved the quality of the thread, but not to a point of being ideal- the smallest moves I could get were about .004" per facet and the result looked like a less than ideal cut finish, because it essentially reflected the curf of the .5" diameter tool on the .004 linear moves.  I would have liked like .001 facets ideally.  These filters could really benefit from the ability to actually smooth a cut by outputting arcs in G12.1.

I then drew a flat arc and used 2D contour.  I posted it to Cimco edit 8, backplotted the G12.1 using fanuc mill to see the arc moves.  Unfortunately the move was comprised of two arc moves in different quadrants in G12.1, so I had to design a compass in Solidworks 2D sketch, extrude that, bring it to a drawing in 1:1 size, print that at the identical diameter to Cimco on the screen (10.490 displayed diameter), and overlap that on the screen with the lights off.  From this I was able to derive the split was ~4 degrees of the arc.  I did math to find the Z of the helix, over the 4 degrees and the other ~63.XXXX degrees and added the Z difference to each G12.1 move of the arc.  This was the highest quality version of the triple index thread I was able to cut using Mastercam, because now it output the arc in an arc move that could helix with the addition of the Z values.  

Hopefully this can help someone until Mastercam can support thread milling on a portion of an arc.  

I guess I also could have gone to the crazy interpolated C diameter derived feeds of Fanuc and attempted to do something, but sometimes the degree callout reverses the rotational direction of the chuck in these cases, so I felt posting it was smarter than standing in the door of the machine with sharpy marker on the part and trial and error posting C moves and going to a calculator to derive the feed moves on the C lines.  Granted if I had known it was going to be as tough, I may have attempted that.  Y axis would have simplified it, but I was trying to balance cutting on a twin path machine.  I ended up making the part in 3:58 run time, with ~ 15 total seconds of imbalanced cutting between the paths.  The balancing was handled in Cimco edit 8 after timing actual cutting.  

I had another C axis G12.1 dynamic milling path cutting 52 seconds, that actually picked up 12 seconds of advantage from G05.1 smoothing settings.  It was the first time I had noticed fanuc smoothing effect a run time.  

[AGreen5]

On 5/13/2020 at 6:55 AM, JParis said:

For the color problem, check this..if it is set to "use group" change it to use "entity colors"

 

 

and check these setting for stock display

I did do the config edit upon seeing your post, before calling Shopware and they were able to tell me this was a parasolid issue with 2020.    The stock display wasn't a solution because my software again was acting strange.  When I drew a box and extruded that to make the stock model, that solid responded normally, so it was simply the bounding box solid which didn't display properly.   I called last week with an issue of toolpath editor not displaying the backplot wires and again it was, "Oh you're lucky to have these odd problems we can't solve."  Which I can appreciate I guess.  I trial and error counted moves to edit feed in a corner in toopath editor blind without the display.  It still worked and I was able to post the file with the slower feed in the corner.    I used it because I wanted to attempt to bring it into the scope of things I understood about the software, and upon initially looking at it I just thought, I think this is supposed to show backplot like geometry which I guess it is supposed to do.  

On 5/13/2020 at 1:30 AM, David Colin said:

Are you sure your chains were drawn at same Cplane? same Z depth?

Post a file if you need help

I think my issue with the chaining was that I had the plane and the clicked Z depth at very slightly different heights so they looked together but were not.  That CAD drawing methodology of select a plane, select a 2D or 3D mode, click Z and click a value for depth, is pretty easy to mess up.  I like the easy Solidworks click sketch, click a face and draw something that looks like a sketch and then dimension and relate it.  Topsolid has even nicer functionality where the drawing scales from the first dimension added- but they ruined that with the forced PDM which hides/takes hostage of the files in a strange storage system in the fragile windows architecture.  If I had a better working knowledge of 3D chaining methods, I could probably use that to sketch less in mastercam.  

Sorry about the post reply strangely appearing here.  I saw this little notification popup and used the reply function on it and that stuff posted here instead of in those native posts. 

[AGreen5]

I guess on the right side of the dialog, in smoothing settings, you can force line moves to be smaller than what Shopware help got me.  I guess I could have gone to .0005" if I wanted.  It wouldn't be as smooth in the control or as fast as the two arc with Z moves I have now, but it would cut with better quality than the original .004" moves.  Not as good as two arcs though, two arcs are smooth moves.  

This is an improvement to thread milling that should exist- the ability to recognize a 2D arc and apply a helix on that move only from the centerpoint for ID or outside for OD threads. 

[gcode]

AGreen5 

I moved this thread to the Industrial Forum

You should get a lot more replies here

This is an interesting topic. Could you upload a non proprietary sample

of the multistart interrupted thread you are trying to machine?

 

[crazy^millman]

Due to the limited information provided here is what I hope will be a help. The process to create a multi lead thread is no different in MT than it is in Mill or Lathe with Mill added on. You create your standard Threadmill Operation. You define your pitch multiplied by X.  X = Number of leads. I have create a simple example here to show you how to go about the process of create a 3 lead thread with a 20 pitch thread. The math is like so. a 3 Lead 20 TPI thread has a.150 pitch for each of the 3 leads. 1/20 = .05 X 3 = .150. Now we need to clock the start point for each thread. 360/3 = 120. Each operation will have a start angle 120 degrees apart from each other. 0, 120 and 240 will be our start angles.  They all share the same Linking parameters. This is important the start angle does the work for the lead of threads. We have a 5 lead thread then we do the match using that lead.

Each operations Toolpath parameter page look like so.

 

 

Here is the verify with Color Loop showing 3 leads.

 

 

Here is a link to a Video showing the toolpath cutting. Backplot Video

Here is the NC code:

N100
(OPERATION # 42)
G91 G0 G28 X0. Y0.
G28 Z0.
M108
G90 G0 B0.
M107
(T004  |  0.25 THREAD MILL  | DIA. -  0.25)
G10.9 X0
M901
M200
T004 M6
G97 S1000 M03
G54
G17
M108 M212
G0 B90. C315.
M107 M210
G68 X0. Y0. Z0. I0. J1. K0. R90.
G43 H4 G0 Z1.5497
X9.7969 Y.0354
Z1.3997
G94 G1 Z.8582 F25.
X9.75 F5.
G3 X9.7969 Y-.0115 Z.877 I.0469 J0. K.0094
X9.8437 Y.0354 Z.8957 I0. J.0469
X9.75 Y.1291 Z.9332 I-.0938 J0. K.0187
X9.6562 Y.0354 Z.9707 I0. J-.0938
X9.75 Y-.0584 Z1.0082 I.0938 J0.
X9.8437 Y.0354 Z1.0457 I0. J.0938
X9.75 Y.1291 Z1.0832 I-.0938 J0.
X9.6562 Y.0354 Z1.1207 I0. J-.0938
X9.75 Y-.0584 Z1.1582 I.0938 J0.
X9.8437 Y.0354 Z1.1957 I0. J.0938
X9.75 Y.1291 Z1.2332 I-.0938 J0.
X9.6562 Y.0354 Z1.2707 I0. J-.0938
X9.75 Y-.0584 Z1.3082 I.0938 J0.
X9.8437 Y.0354 Z1.3457 I0. J.0938
X9.75 Y.1291 Z1.3832 I-.0938 J0.
X9.6597 Y.0606 Z1.4142 I0. J-.0938 K.0155
X9.658 Y.048 Z1.4175 I.0451 J-.0126 K.0016
X9.7049 Y.0011 Z1.4362 I.0469 J0. K.0094
X9.75 Y.0354 Z1.4517 I0. J.0469 K.0077
G1 X9.7049 Y.048
G0 Z1.5497
G69
G49

(OPERATION # 43)
G54
G17
G68 X0. Y0. Z0. I0. J1. K0. R90.
G43 H4 G0 X9.7266 Y.076 Z1.5497
Z1.3997
G94 G1 Z.8582 F25.
X9.75 Y.0354 F5.
G3 X9.7734 Y.076 Z.8707 I-.0234 J.0406 K.0062
X9.7266 Y.1228 Z.8895 I-.0469 J0. K.0094
X9.7031 Y.1165 Z.8957 I0. J-.0469 K.0031
X9.6562 Y.0354 Z.9207 I.0469 J-.0812 K.0125
X9.75 Y-.0584 Z.9582 I.0938 J0. K.0188
X9.8437 Y.0354 Z.9957 I0. J.0938
X9.75 Y.1291 Z1.0332 I-.0938 J0.
X9.7031 Y.1165 Z1.0457 I0. J-.0938 K.0062
X9.6562 Y.0354 Z1.0707 I.0469 J-.0812 K.0125
X9.75 Y-.0584 Z1.1082 I.0938 J0. K.0188
X9.8437 Y.0354 Z1.1457 I0. J.0938
X9.75 Y.1291 Z1.1832 I-.0938 J0.
X9.7031 Y.1165 Z1.1957 I0. J-.0938 K.0062
X9.6562 Y.0354 Z1.2207 I.0469 J-.0812 K.0125
X9.75 Y-.0584 Z1.2582 I.0938 J0. K.0188
X9.8437 Y.0354 Z1.2957 I0. J.0938
X9.75 Y.1291 Z1.3332 I-.0938 J0.
X9.7031 Y.1165 Z1.3457 I0. J-.0938 K.0062
X9.6562 Y.0354 Z1.3707 I.0469 J-.0812 K.0125
X9.75 Y-.0584 Z1.4082 I.0938 J0. K.0188
X9.7733 Y-.0554 Z1.4142 I0. J.0938 K.003
X9.8085 Y-.01 Z1.43 I-.0117 J.0454 K.0079
X9.7617 Y.0368 Z1.4487 I-.0469 J0. K.0094
X9.75 Y.0354 Z1.4517 I0. J-.0469 K.0015
G1 X9.7617 Y-.01
G0 Z1.5497
G69
G49

(OPERATION # 44)
G54
G17
G68 X0. Y0. Z0. I0. J1. K0. R90.
G43 H4 G0 X9.7266 Y-.0052 Z1.5497
Z1.3997
G94 G1 Z.8582 F25.
X9.75 Y.0354 F5.
G3 X9.7266 Y.0416 Z.8645 I-.0234 J-.0406 K.0031
X9.6797 Y-.0052 Z.8832 I0. J-.0469 K.0094
X9.7031 Y-.0458 Z.8957 I.0469 J0. K.0062
X9.75 Y-.0584 Z.9082 I.0469 J.0812
X9.8437 Y.0354 Z.9457 I0. J.0937 K.0188
X9.75 Y.1291 Z.9832 I-.0938 J0.
X9.6562 Y.0354 Z1.0207 I0. J-.0937
X9.7031 Y-.0458 Z1.0457 I.0938 J0. K.0125
X9.75 Y-.0584 Z1.0582 I.0469 J.0812 K.0062
X9.8437 Y.0354 Z1.0957 I0. J.0937 K.0188
X9.75 Y.1291 Z1.1332 I-.0938 J0.
X9.6562 Y.0354 Z1.1707 I0. J-.0937
X9.7031 Y-.0458 Z1.1957 I.0938 J0. K.0125
X9.75 Y-.0584 Z1.2082 I.0469 J.0812 K.0062
X9.8437 Y.0354 Z1.2457 I0. J.0937 K.0188
X9.75 Y.1291 Z1.2832 I-.0938 J0.
X9.6562 Y.0354 Z1.3207 I0. J-.0937
X9.7031 Y-.0458 Z1.3457 I.0938 J0. K.0125
X9.75 Y-.0584 Z1.3582 I.0469 J.0812 K.0063
X9.8437 Y.0354 Z1.3957 I0. J.0937 K.0188
X9.817 Y.1009 Z1.4142 I-.0938 J0. K.0092
X9.7835 Y.115 Z1.4237 I-.0335 J-.0328 K.0048
X9.7366 Y.0682 Z1.4425 I0. J-.0469 K.0094
X9.75 Y.0354 Z1.4517 I.0469 J0. K.0046
G1 X9.7835 Y.0682
G0 Z1.5497
G69
G49
G91 G28 X0. Y0.
G28 Z0. M05
M108
G90 G0 B0.
M107
M999
M30

G109 L2 (LOWER TURRET)
M999
M30

Now no sample was given only the mention of G12.1 so you are trying to do this with C axis only in a cross slide configuration then I can see your issue. If trying to do in the face of part with Z tool then the above should still work.

Link to summary of this Response with Pictures

Edited June 4, 2021 by crazy^millman
Reduce Attachments to allow for future help