topic Re: post processor siemens in HSM Post Processor Forum

post processor siemens

Anonymous — Wed, 22 Jul 2020 17:23:18 GMT

Salve

Per favore qualcuno potrebbe aiutarmi a modificare questo post :

Siemens Turning / Siemens Turning

Grazie

Simone

Questo è il post originale :

; %_N_30_MPF
N10 G90 G94 G18
N11 G71
N12 LIMS=6000
N13 G53 G0 X0.
( SFACCIATURA )
N14 T5 D1
N15 G54
N16 M8
N17 G95
N18 G97 S637 M4
N19 G0 X100. Z5
N20 G96 S200 M4
N21 LIMS=5000
N22 G0 Z1.414
N23 X92.
N24 G1 X94.828 F0.15
N25 X92. Z0
N26 X25.4
N27 X28.228 Z1.414
N28 G0 X100.
N29 Z5
N30 G97 S637 M4
( SGROSSATURA )
N31 G95
N32 G97 S624 M4
N33 G0 X102. Z5
N34 G96 S200 M4
N35 LIMS=5000
N36 G0 Z3
N37 X93.
N38 G1 Z-24.8 F0.2
N39 X99.
N40 G0 Z3
N41 X87.2
N42 G1 Z-24.8 F0.2
N43 X93.
N44 X95. Z-23.8
N45 G0 Z3
N46 X81.399
N47 G1 Z0 F0.2
N48 G18 G3 X84.999 Z-1.8 K-1.8
N49 G1 Z-24.8
N50 X87.2
N51 X89.2 Z-23.8
N52 G0 X99.
N53 Z3
N54 X102.
N55 Z5
N56 G97 S624 M4
N57 M9
N58 G53 X0.
( FINITURA )
N59 M1
N60 T3 D1
N61 G54
N62 M8
N63 G95
N64 G97 S624 M4
N65 G0 X102. Z5
N66 G96 S200 M4
N67 LIMS=5000
N68 G0 Z1.414
N69 X86.012
N70 G1 X79.371 F0.15
N71 X82.199 Z0
N72 G18 G3 X84.999 Z-1.4 K-1.4
N73 G1 Z-24.4
N74 X88.999
N75 G0 X102.
N76 Z5
N77 G97 S624 M4
N78 M9
N79 G53 X0.
N80 G53 Z0
N81 M30

Questo è il post modificato che vorrei :

In blu ho messo come inizia e finisce prima di un cambio utensile.

%MPF30
N14 T5 D5 ( ESTERNO CNMG 08 )
N15 G54
N16 G96 S200 M3 M8 F0.15
N17 G92 S3000
N19 G0 X100. Z5
N22 G0 Z1.414
N23 X92.
N24 G1 X94.828
N25 X92. Z0
N26 X25.4
N27 X28.228 Z1.414
N28 G0 X100.
N29 Z5
N33 G0 X102. Z5
N36 G0 Z3
N37 X93.
N38 G1 Z-24.8 F0.2
N39 X99.
N40 G0 Z3
N41 X87.2
N42 G1 Z-24.8 F0.2
N43 X93.
N44 X95. Z-23.8
N45 G0 Z3
N46 X81.399
N47 G1 Z0 F0.2
N48 G3 X84.999 Z-1.8 K-1.8 ( RIMUOVERE IL G18 )
N49 G1 Z-24.8
N50 X87.2
N51 X89.2 Z-23.8
N52 G0 X99.
N53 Z3
N54 X102.
N55 Z5
G0 X300 Z300 M9
N60 T1 D1 ( ESTERNO DNMG 04 )
G54
G96 S200 M3 M8 F0.15
G92 S3000
N65 G0 X102. Z5
N68 G0 Z1.414
N69 X86.012
N70 G1 X79.371 F0.15
N71 X82.199 Z0
N72 G18 G3 X84.999 Z-1.4 K-1.4
N73 G1 Z-24.4
N74 X88.999
N75 G0 X102.
N76 Z5
G0 X300 Z200 M9
M5 M30

Re: post processor siemens

KrupalVala — Wed, 29 Jul 2020 07:03:18 GMT

Hi @Anonymous ,

You can change/control spindle rotation direction, Constant surface speed on-off ,feederate unit, and etc through Fusion360 project.

Also you can give home/safe position while posting the codes.

Re: post processor siemens

Anonymous — Thu, 30 Jul 2020 21:17:14 GMT

Thank you so much for your answer Krupa.Vala
I tried to put the value 300 on the g53 but when I do the post I don't see that it has changed anything.
I have improved other parts but I needed it to go to X300 and Z300 at every tool change
The post I would like to get is like the one I published earlier. 
If you have any other tips I would be happy, thanks goodnight

Re: post processor siemens

KrupalVala — Sun, 02 Aug 2020 11:41:10 GMT

Hi @Anonymous ,

To get the X and Z safe home position, you just need to remove // from below given location .

Open your post in any editor, search below codes and change these codes......

if (insertToolCall || newSpindle || newWorkOffset) { // retract to safe plane retracted = true; if (!isFirstSection() && insertToolCall) { onCommand(COMMAND_COOLANT_OFF); } writeBlock(gAbsIncModal.format(90), gFormat.format(53), gMotionModal.format(0), "X" + xFormat.format(properties.g53HomePositionX)); // retract // writeBlock(gAbsIncModal.format(90), gFormat.format(53), gMotionModal.format(0), "Z" + zFormat.format(properties.g53HomePositionZ)); // retract, optional forceXYZ(); }

To these one.

if (insertToolCall || newSpindle || newWorkOffset) { // retract to safe plane retracted = true; if (!isFirstSection() && insertToolCall) { onCommand(COMMAND_COOLANT_OFF); } writeBlock(gAbsIncModal.format(90), gFormat.format(53), gMotionModal.format(0), "X" + xFormat.format(properties.g53HomePositionX)); // retract writeBlock(gAbsIncModal.format(90), gFormat.format(53), gMotionModal.format(0), "Z" + zFormat.format(properties.g53HomePositionZ)); // retract, optional forceXYZ(); }

Save he post and test it. Also, you can learn and modified the post postprocessor from a Post Processor Training Guide . It is designed to be used by both beginners, advanced post users and developers.

Thanks,

Re: post processor siemens

Anonymous — Sun, 02 Aug 2020 14:13:13 GMT

Thanks Krupa.Vala
I solved this problem.
I would also have this problem, I would like to eliminate g95 g97 and make sure that at each tool change there is no longer this:

N1 T5 D1
N6 G54
N11 M8
N16 G95
N21 G97 S0 M4
N26 G90 G0 X162. Z5
N31 G96 S200 M4

but this

%MPF30
N14 T5 D5 ( ESTERNO CNMG 08 )
N15 G54
N16 G96 S200 M3 M8 F0.15
N17 G92 S3000
N19 G0 X162. Z5

and make sure that t as the number corresponds to D
that is, no longer
T1 D6
but
T1 D1
T2 D2
T3 D3
Thanks in advance good day

Re: post processor siemens

Anonymous — Sun, 02 Aug 2020 14:17:35 GMT

and eliminate the g18

N296 G18 G3 X125.999 Z-2.8 I-2.301 K-1.766

Re: post processor siemens

KrupalVala — Sun, 02 Aug 2020 18:35:19 GMT

Hi @Anonymous ,

To get desired "D" compensation Offset, You need to modify the post as shown below and have to control those Number through Fusion360 only.

1.1)

Open your post in any editor and search below codes (inside the insertToolCall)

var compensationOffset = 1; // optional, use tool.isTurningTool() ? tool.compensationOffset : tool.lengthOffset if (compensationOffset > 99) { error(localize("Compensation offset is out of range.")); return; } writeBlock("T" + toolFormat.format(tool.number), dFormat.format(compensationOffset)); if (tool.comment) { writeComment(tool.comment); }

and set it to....

var compensationOffset = tool.isTurningTool() ? tool.compensationOffset : tool.lengthOffset if (compensationOffset > 99) { error(localize("Compensation offset is out of range.")); return; } writeBlock("T" + toolFormat.format(tool.number), dFormat.format(compensationOffset)); if (tool.comment) { writeComment(tool.comment); }

1.2) Open your fusion project. Go to tool library and set compensation number same as tool number as shown below image.

T3 D3 - set offset number inside the tool

Note : T3(Number) D3 (Compensation offset) - set offset number inside the tool

2) To Eliminate g95 g97, Go to function getCode(code) { .

Add // to ignore those codes as show below,

case "FEED_MODE_UNIT_REV": return //gFeedModeModal.format(95); case "FEED_MODE_UNIT_MIN": return gFeedModeModal.format(94); case "CONSTANT_SURFACE_SPEED_ON": return gSpindleModeModal.format(96); case "CONSTANT_SURFACE_SPEED_OFF": return //gSpindleModeModal.format(97);

3) G18 is depend on your toolpath. You can control it through fusion360.

Now save the post and test it carefully.

Thanks,

Re: post processor siemens

Anonymous — Sun, 02 Aug 2020 20:28:55 GMT

Krupa.Vala you have solved everything for me, now I will try it but I am already very satisfied.
thanks again goodnight

Re: post processor siemens

KrupalVala — Mon, 03 Aug 2020 05:19:19 GMT

Hi @Anonymous ,

Thank you for your feedback. 🙂

Regards,

Re: post processor siemens

Anonymous — Mon, 03 Aug 2020 12:52:13 GMT

Good morning, Krupal Vala
I have one more thing left to remove in the post. The line N216 S0 M3 I wish it wasn't there because the spindle stops me

N1 T5 D5

N6 G54

N11 M8

N16 G90 G0 X123. Z5

N21 G96 S200 M3

N26 G0 Z4.214

N31 X103.

N36 G1 X95.828 F0.15

N41 X93. Z2.8

N46 X17.4

N51 X20.228 Z4.214

N56 G0 X103.

N61 Z3.714

N66 G1 X95.828 F0.15

N71 X93. Z2.3

N76 X17.4

N81 X20.228 Z3.714

N86 G0 X103.

N91 Z3.214

N96 G1 X95.828 F0.15

N101 X93. Z1.8

N106 X17.4

N111 X20.228 Z3.214

N116 G0 X103.

N121 Z2.714

N126 G1 X95.828 F0.15

N131 X93. Z1.3

N136 X17.4

N141 X20.228 Z2.714

N146 G0 X103.

N151 Z2.214

N156 G1 X95.828 F0.15

N161 X93. Z0.8

N166 X17.4

N171 X20.228 Z2.214

N176 G0 X103.

N181 Z1.714

N186 G1 X95.828 F0.15

N191 X93. Z0.3

N196 X17.4

N201 X20.228 Z1.714

N206 G0 X123.

N211 Z5

N216 S0 M3 ---------------------------------------- ( to be deleted if possible )

Thanks in advance

Re: post processor siemens

KrupalVala — Mon, 03 Aug 2020 18:02:47 GMT

Hi @Anonymous ,

Could you please share you Fusion360 project? So I can check the issue and let you know.

Thanks,

Re: post processor siemens

Anonymous — Mon, 03 Aug 2020 19:44:20 GMT

by project do you mean the right postprocessor config file?

Re: post processor siemens

KrupalVala — Mon, 03 Aug 2020 20:12:07 GMT

Hi @Anonymous ,

I meant to say Your Fusion360 "CAM" project. Also share your post config file.

Thanks,

Re: post processor siemens

Anonymous — Mon, 03 Aug 2020 20:27:33 GMT

Re: post processor siemens

KrupalVala — Tue, 04 Aug 2020 04:40:38 GMT

Hi @Anonymous ,

Your CAM project is ok. Could you please share your post processor / .cps file to me?

Thanks,

Re: post processor siemens

Anonymous — Tue, 04 Aug 2020 06:35:13 GMT

Sure, can I make a copy and paste or is there a way to share the file?
Thank you

Re: post processor siemens

KrupalVala — Tue, 04 Aug 2020 06:47:40 GMT

Hi @Anonymous ,

Please compress the file then Drag & drop it in the attachment area.

Re: post processor siemens

Anonymous — Tue, 04 Aug 2020 06:58:46 GMT

Thank you
I attached the cps file, attracting your info

Re: post processor siemens

KrupalVala — Tue, 04 Aug 2020 07:37:29 GMT

Hi @Anonymous

I have check your post and found one major issue. You have ignored Speedle start. due to that you are not getting RMP at any level.

startSpindle(false, true, initialPosition);

For the post-processor learning and modification, you can refer a Post Processor Training Guide manual and edit posts isn't difficult once you've got started. Click here to Download Guide

Thanks,

Re: post processor siemens

Anonymous — Tue, 04 Aug 2020 12:49:55 GMT

Hi Krupal Vala
I don't know why this command was ignorant, anyway I removed // but I didn't have any results.
anyway as you say I'll try to take a look at the post guide that you linked to me.
Thanks for the reply and good day