Tormach SFM and IPR modes on mill turning

[TomD]

This is probably more appropriate in a new post than me necro'ing a thread.  I used my Tormach PCNC 1100 with Fusion 360 today to do some mill turning for the first time.  Since I had SFM and IPR turned on in fusion I got a G1 F0 error AND a spindle stopped error.  I fixed the errors and ran the part using RPM and IPM in fusion to get a correct NC file BUT I can't see any reason G95 and G96 cannot be used.  I modified an NC file (shown below) and ran it in path pilot simulation and it all seems to work ok.  Can someone tell me either why I shouldn't do this, or if I should how to go about editing my post?

%
(1001)
(T49  D=0. CR=0. - ZMIN=-3.1095 - general turning)
G90 G54 G64 G50 G17 G40 G80 G95 G91.1 G49
G96 D5000 S400
G20 (Inch)
G30

N10(Profile Roughing1)
T49 G43 H0 M6
M3 M8 
G54
G0 X0.9 Y0.
G0 Z0.1969
G0 Z-0.0457
G0 X0.4767
G1 Z-3.1095 F0.
G1 X0.5
G1 X0.54 Z-3.0695
G0 Z-0.0457
G0 X0.4535
G1 Z-3.1095 F0.
G1 X0.4767
G1 X0.5167 Z-3.0695
G0 Z-0.0457
G0 X0.4302
G1 Z-3.1095 F0.
G1 X0.4535
G1 X0.4935 Z-3.0695
G0 Z-0.0457
G0 X0.407
G1 Z-3.1095 F0.
G1 X0.4302
G1 X0.4702 Z-3.0695
G0 Z-0.0457
G0 X0.3837
G1 Z-3.1095 F0.
G1 X0.407
G1 X0.447 Z-3.0695
G0 Z-0.0457
G0 X0.3598
G1 Z-2.5737 F0.
G1 X0.3837
G1 X0.4237 Z-2.5337
G0 Z-0.0457
G0 X0.3359
G1 Z-2.5737 F0.
G1 X0.3598
G1 X0.3998 Z-2.5337
G0 Z-0.0457
G0 X0.312
G1 Z-2.5737 F0.
G1 X0.3359
G1 X0.3759 Z-2.5337
G0 Z-0.0457
G0 X0.2881
G1 Z-2.5737 F0.
G1 X0.312
G1 X0.352 Z-2.5337
G0 Z-0.0457
G0 X0.2595
G1 Z-1.2519 F0.
G1 X0.2651 Z-1.258
G1 Z-1.8655
G1 X0.2738
G1 Z-2.0029
G1 X0.2655 Z-2.0094
G1 Z-2.4036
G1 X0.2881
G1 X0.3281 Z-2.3636
G0 Z-0.0457
G0 X0.2309
G1 Z-0.728 F0.
G1 X0.2539
G1 Z-0.8104
G1 X0.2309 Z-0.8283
G1 Z-0.8391
G1 X0.2539
G1 Z-0.9214
G1 X0.2309 Z-0.9394
G1 Z-1.2203
G1 X0.2595 Z-1.2519
G1 X0.2995 Z-1.2119
G0 Z-0.0457
G0 X0.207
G1 Z-0.728 F0.
G1 X0.2309
G1 X0.2709 Z-0.688
G0 Z-0.0457
G0 X0.1831
G1 Z-0.7276 F0.
G1 X0.1867 Z-0.7279
G1 X0.1904 Z-0.728
G1 X0.207
G1 X0.247 Z-0.688
G0 Z-0.0457
G0 X0.1591
G1 Z-0.7183 F0.
G18 G2 X0.1831 Z-0.7276 I0.0312 K0.0455
G1 X0.2231 Z-0.6876
G0 Z-0.0457
G0 X0.1495
G1 X0.1352 F0.
G1 Z-0.6729
G2 X0.1591 Z-0.7183 I0.0552 K0.
G1 X0.1991 Z-0.6783
G0 X0.2682
G0 Z-0.8283
G0 X0.2452
G1 X0.2309 F0.
G1 X0.2172 Z-0.8391
G1 X0.2309
G1 X0.2709 Z-0.7991
G0 Z-0.9394
G0 X0.2452
G1 X0.2309 F0.
G1 X0.2096 Z-0.956
G1 Z-1.2026
G1 X0.2127 Z-1.2032
G1 X0.2158 Z-1.2037
G1 X0.2309 Z-1.2203
G1 X0.2709 Z-1.1803
G0 Z-0.956
G0 X0.2239
G1 X0.2096 F0.
G1 X0.1884 Z-0.9726
G1 Z-1.1924
G2 X0.2096 Z-1.2026 I0.0339 K0.0435
G1 X0.2496 Z-1.1626
G0 Z-0.9726
G0 X0.2027
G1 X0.1884 F0.
G1 X0.1671 Z-0.9892
G1 Z-1.1489
G2 X0.1884 Z-1.1924 I0.0552 K0.
G1 X0.2284 Z-1.1524
G0 X0.5143
G0 Z-0.0457
G0 X0.9
G0 Z0.1969
G17
M5 M9

G30
M30
%

[bob.schultz]

Hello @TomD,

Are you using the RapidTurn attachment on your Tormach mill?  If so, you should use the Tormach Turning (PathPilot) post processor instead of the mill post processor.

If you are turning a part in the milling spindle, then you will need to add the capabilities to the post yourself.  To add G95 support, you can add a property (Use G95) as is present in the Fanuc post processor.  Search for useG95 in the post and modify your post to include this logic.  Another option is to copy the logic from the Tormach Turning post, search for FEED_MODE_UNIT_REV in this post.  You will also need to increase the accuracy of the F-code to support FPR feedrates, so you do not get F0 output.

  var feedFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true});

Concerning G96 support, even if the control supports G96 it will probably not work for turning on a mill, since the control will use the full diameter of the tool (part) to calculate the RPM speed and not the depth of the cut from a part loaded in the spindle and a fixed tool.

[TomD]

I'm turning in the mill spindle itself with a homemade lathe tool block.

I managed to get the feed to 3 decimals, the rest of the G95 is eluding me at the moment but I am working on it.  I added a property, its just a matter of figuring out the interaction between what Fusion is showing the post processor so I can flesh out the rest.  I've not modified any post previously but am pretty decent with JS and python so I think I can get there.

As for G96, Tormach interprets based on the distance from X0 so the RPM increases/decreases as you would expect.    Im using a WCS for each tool and the work as always the same tool number so this has the desired effect.  I confirmed that a little bit ago.  Getting the post to actually spit it out without manually adding it is another story.  The cheater way is to just use if spindle_speed == 0 and replace the text there.

[TomD · Accepted solution]

Additionally, there is a flag in the Tormach TURNING post that you can turn to true for turning in the spindle which solves all of these issues aside from manually having to add WCS before changing tools. I found it while digging for the other options

[bob.schultz]

Yes, I forgot we left this in the post.  Glad to hear it is working for you.