Siemens 810t L97 Cycle working but..

robert_persson · ‎07-20-2018

Hi, Got the L97 Cycle working but need some help Tweaking it

I need some pointers how to get the finish and start point in Z.

This is the code im using now to get the start and finish point!

var backFromFront = hasParameter("operation:applyStockOffsetBackFromFront") && getParameter("operation:applyStockOffsetBackFromFront") === 1;
var pos = backFromFront ? currentSection.getFinalPosition() : currentSection.getInitialPosition();
var ThreadFinishPointZ = backFromFront ? pos.z : z;

ThreadStartPointZ = ThreadFinishPointZ + -cycle.incrementalZ;

Im not getting the precise start and stop values with this code im a few tenths of a millimetre off.

It shouldnt be any big problems converting the threading cycle to other Siemens machines when im done.

Can someone please give me some pointers??

robert_persson · ‎07-21-2018

Have figured out that it has to do with the pitch...

When i have the pitch set to 2mm then the z start and finish point is zero.

This is how it looks.

1001
N1 G90 G94 G18
N2 G71
N3 G92 S3500

( Thread2 )
N29 G95
N30 G97 S500 M4
N31 G0 X62 Z5
N32 G0 Z0
(R20 = 2 Pitch)
(R21 = 60 Start point of the thread in X)
(R22 = 0 Start point of the thread in Z)
(R23 = 0 Number of idle passes)
(R24 = -1.3 Thread depth (positive value = inside thread, negative value = outside thread))
(R25 = 0.05 Finishing increment)
(R26 = 0 Approach Path)
(R27 = 0 Run-Out Path)
(R28 = 5 Number of roughing cuts)
(R29 = 0 Infeed Angle)
(R31 = 60 End point of the thread in X (absolute))
(R32 = -20 End point of the thread in z (absolute))
N33 R20=2 R21=60 R22=0 R23=0 R24=-1.3 R25=0.05 R26=0 R27=0 R28=5 R29=0 R31=60 R32=-20
N34 L97 P1
N35 G0 Z5

N64 M9
N65 M30
%

This is the z start point with different pitch values.

(R20 = 0.5 Pitch)
(R22 = 0.344 Start point of the thread in Z)

(R20 = 1 Pitch)
(R22 = 0.229 Start point of the thread in Z)

(R20 = 1.5 Pitch)
(R22 = 0.115 Start point of the thread in Z)

(R20 = 2 Pitch)
(R22 = 0 Start point of the thread in Z)

(R20 = 2.5 Pitch)
(R22 = -0.115 Start point of the thread in Z)

(R20 = 3 Pitch)
(R22 = -0.229 Start point of the thread in Z)

(R20 = 3.5 Pitch)
(R22 = -0.344 Start point of the thread in Z)

(R20 = 4 Pitch)
(R22 = -0.458 Start point of the thread in Z)

The difference seems "linear" so it should be possible to correct with some calculations but how ? 😉

robert_persson · ‎07-22-2018

Its solved now with the help with some Math!

This is how it looks now!

( Thread0,5 )
N4 T2 D2
( OD Threading )
N5 G54
N6 G58 Z60
N7 M8
N8 G95
N9 G97 S500 M4
N10 G0 X62 Z5.344
N11 G0 Z1.932
(R20 = 0.5 Pitch)
(R21 = 60 Start point of the thread in X)
(R22 = 0 Start point of the thread in Z)
(R23 = 0 Number of idle passes)
(R24 = -1.3 Thread depth (positive value = inside thread, negative value = outside thread))
(R25 = 0.05 Finishing increment)
(R26 = 1 Approach Path)
(R27 = 2 Run-Out Path)
(R28 = 5 Number of roughing cuts)
(R29 = 29.5 Infeed Angle)
(R31 = 60 End point of the thread in X (absolute))
(R32 = -20 End point of the thread in z (absolute))
N12 R20=0.5 R21=60 R22=0 R23=0 R24=-1.3 R25=0.05 R26=1 R27=2 R28=5 R29=29.5 R31=60 R32=-20
N13 L97 P1
N14 G0 Z5.344

N15 M9
N16 M30

Anonymous · ‎07-14-2019

@robert_persson would you mind posting a copy of your post processor? I am working on a EMCO 320 lathe with an 810T control and having some issues. for one, the canned threading cycle is not working, but it looks like you might have found the solution.

Is your post processor working with the drilling canned cycles? Mine is not because it is not calling the right R values, and I'm not quite proficient enough to tweak the post processor. I'd love to see a copy of yours because it sounds like you may have solved this?

robert_persson · ‎07-15-2019

Hi, you can try it out, i think the L98 cycle for deep hole drilling is working.

Anonymous · ‎07-15-2019

Great, thank you for the fast response! I'll give this a shot and see what happens.

Anonymous · ‎07-15-2019

Hey @robert_persson I think I must have misunderstood this thread. I thought that you had figured out a way that you could have Fusion 360 take the thread information and use the post processor to turn it into R values so that threading would happen as a canned L97 cycle. But after examining the post processor, I don't think it acts that way.

I too can get the L97 threading to work by manually inserting the code with the proper R values, but have not figured out a way to make this work within Fusion 360.

Let me know if I'm off base.

Thanks for sending me your post processor. I'm still having an issue with drilling. Your post calls up drilling as "CYCLE81" where as mine is looking for a canned cycle. But I might be able to hack my post together to make it work.

robert_persson · ‎07-15-2019

Hi,

That was strange,

I tested with a newly installed fusion and i had to turn off and on threading cycle first before it worked.

%MPF111
( program: %MPF111 )
( NaN )
( undefined )
( Generated at: 2019/7/16 7:16:43 on N55SF )
( Postprocessor: D:\Dokument\OwnCloud\CNC\Postprocessors\Fusion360\Siemens\EMCO_810T_2018-07-23.cps )
( Cam: Fusion 360 CAM 2.0.6037 )
N1 G90 G94 G18
N2 G71
N3 G92 S3500

( Drill2 )
N4 T5 D5
N5 G54
N6 G58 Z60
N7 G94
N8 G97 S810 M3
N9 G0 X0 Z4
N10 F49
N11 R11=0 R22=8.995 R24=1.5 R25=1.5 R26=-22.445 R27=0 R28=0
N12 L98 P1
N13 G0 X0 Z8.995
N14 G0 Z4

( Thread1 )
N15 M1
N16 T6 D6
N17 G54
N18 G58 Z60
N19 M8
N20 G95
N21 G97 S500 M3
N22 G0 X14 Z25
N23 G0 Z3.751
N24 R20=1 R21=12.2 R22=-1.642 R23=1 R24=0.535 R25=0.05 R26=5 R27=1 R28=5 R29=29 R31=12.2 R32=-14.029
N25 L97 P1
N26 G0 Z25

N27 M9
N28 M30
%

Now i get this output!

Program name must start with %MPF.

You can turn off cycle comments, notes and postinformation with the program settings property window.

Anonymous · ‎07-16-2019

I tried this a couple times with no luck... and then, MAGIC!!!! The clouds parted, a choir started singing, and Fusion 360 posted this beautiful code:

%MPF12
( program: %MPF12 )
( undefined )
( Generated at: 2019/7/16 12:04:17 on WOPR-10 )
( Postprocessor: c:\users\curt\appdata\roaming\autodesk\fusion 360 cam\posts\EMCO_810T_2018-07-23.cps )
( Document: test piece drilling and od threading v1 )
( Cam: Fusion 360 CAM 2.0.6037 )
( Machine )
( vendor: EMCO )
( model: 320 )
( description: EMMA Evaluation Lathe 2019 )
N10 G90 G94 G18
N11 G70
N12 G92 S4000

( Drill1 )
N13 T7 D7
N14 G54
N15 G58 Z60
N16 M8
N17 G94
N18 G97 S410 M4
N19 G0 X0 Z0.75
N20 F2
(L98 Deep hole drilling cycle with chip removal Full retract)
(R11 = 1 (0=With chip breaking, 1=With chip removal)
(R22 = 0.25 Starting point in Z (absolute)
(R24 = 0.1172 Amount of degression (incremental) without sign)
(R25 = 0.1172 The first drilling depth (incremental) without sign)
(R26 = -2 Final drilling depth (absolute)
(R27 = 0 Dwell time at the starting point (for chip removal)
(R28 = 0 Dwell time at the bottom of drilling hole (chip breaking)
N21 R11=1 R22=0.25 R24=0.1172 R25=0.1172 R26=-2 R27=0 R28=0
N22 L98 P1
N23 G0 X0
N24 G0 Z0.25
N25 G0 Z0.75

( Thread2 )
N26 M1
N27 T0 D0
N28 G54
N29 G58 Z60
N30 G95
N31 G97 S500 M3
N32 G0 X2.829 Z0.16
N33 G0 Z0.3937
(R20 = 0.07874015748031496 Pitch)
(R21 = 1.989 Start point of the thread in X)
(R22 = -0.4403 Start point of the thread in Z)
(R23 = 0 Number of idle passes)
(R24 = -0.04 Thread depth (positive value = inside thread, negative value = outside thread))
(R25 = 0.05 Finishing increment)
(R26 = 0.39370078740157477 Approach Path)
(R27 = 0 Run-Out Path)
(R28 = 5 Number of roughing cuts)
(R29 = 0 Infeed Angle)
(R31 = 1.989 End point of the thread in X (absolute))
(R32 = -2.5403 End point of the thread in z (absolute))
N34 R20=0.07874015748031496 R21=1.989 R22=-0.4403 R23=0 R24=-0.04 R25=0.05 R26=0.39370078740157477 R27=0 R28=5 R29=0 R31=1.989 R32=-2.5403
N35 L97 P1
N36 G0 Z0.16

N37 M9
N38 G53 G0 X0 Z0
N39 M30
%

holy smokes! I'm not 100% sure if it works yet, but it's a million steps in the right direction! I'm going to brush up on my javascript skills and start working through this. Thank you! this may be the answer to my problems! Not only did it do the threading correctly with R values, it also did the drilling cycle correctly.

@kanpowersports you need to check this out if you're still working on your lathe!

Anonymous · ‎07-17-2019

for anyone following along with an EMCO 320 Lathe like mine, my post processor is attached. it's not quite final, but is now working with canned cycles, tool retracts before changes, threading, and profiling all operational.

pawel.piela1 · ‎12-14-2019

Hello,

Thanks for sharing your postprocessor.

I'm working on lathe with Pronum 630t control. Its using the same cycles and codes as Sinumerik 810t do, but there are a few differences.

I changed few things but there is one I have no idea how to deal with. After each toolchange there is workoffset number. I want to have work it only in the beginning of program. How to change it?

Anonymous · ‎12-15-2019

It's outside of my comfort zone to give advice here because I'm not very good at modifying post processors. But generally speaking, I'd suggest that you should just look at the post processor and find where it inserts that workoffset number after each toolchange. You can just delete the work offset call after toolchange.

Though, unless it's causing some kind of problem, I'd probably leave it in.

Community

Siemens 810t L97 Cycle working but..

Siemens 810t L97 Cycle working but..

Siemens 810t L97 Cycle working but..