Turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Siemens PLM Community
- NX Manufacturing
- Discussion Forum - NX Manufacturing
- A CSE question?

Options

- Start Article
- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-28-2018 10:09 PM

Hello, I have a machine and simulate machine code file:

PLANE RESET STAY

M129

TOOL CALL 1 Z S6000 DL0.0

CYCL DEF 247 DATUM SETTING Q339=+1 ;DATUM NUMBER

PLANE SPATIAL SPA0.0 SPB-37.38 SPC72. TURN FMAX SEQ+

L X0 Y0 Z0 F1000

Result is:

I would like to make tool position to go to MCS(0,0,0). How can I do it?

Solved! Go to Solution.

7 REPLIES 7

Re: A CSE question?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-29-2018 03:37 AM - edited 05-29-2018 03:42 AM

As I see on right picture you already are on x0y0z0. It is OK. Machine did it correctly.

Actual active MCS is in the midle of purple face.

This is how tilded plane works. Zero point is where it was indicated, only direction is changing.

But in this case we dont see this transformation.

If you mean 000 on highlited mcs on the right picture you have to disable plane or tcpm.

---------------------------------------------

#♫ PB, 5ax, itnc, nx, vericut ♫ #

#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: A CSE question?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-29-2018 04:36 AM

Thank you for your reply.

I am a bit confused. I want to machine the right side of the tool on right picture. NC code like:

L X+44.5073 Y+2.0734

L X+44.5079 Y+2.0734 Z-7.9621

L Z-8.9621 F1000.

L X+36.7579

L X+35.5079 Y+6.9146 Z-8.9622

L X+35.5018 Y+6.9381

L X+31.9036 Y+9.0156

L X+35.5079 Y-4.9439

You can find the face that is under MCS. The NC code is Z-8.9622. If you are right, then NC code Z value should be +Z?.

This becomes a post processor error. But my post processor on CNC is correct.

I have found that the result of the NC code output from my post processor is that the origin of the coordinate will not follow the rotation, but the axis will rotate due to the rotation.

What's this problem? CSE? Post-Processor?

How can I correct it?

Sam Huang

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-29-2018 05:00 AM - edited 05-29-2018 05:05 AM

better will be to attach the part and see operations

now I dont know what you wan to achieve and where is the problem

"I want to machine the right side of the tool on right picture"

Another thing machine simulation can overide postprocesor kinematics etc

but we dont know if it is a problem in this case.

Or there can be problem with zero point settting with cycle 247, dont know. I am not into simulation so much.

attach the prt

---------------------------------------------

#♫ PB, 5ax, itnc, nx, vericut ♫ #

#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: A CSE question?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-29-2018 05:35 AM

Re: A CSE question?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-29-2018 06:45 AM - edited 05-29-2018 06:57 AM

This is my output:

39 PLANE SPATIAL SPA+14.4888 SPB+34.8393 SPC-83.6611 TURN FMAX TABLE ROT

40 L X-3.6621 Y-1.9307

41 L Z+102.9597 FMAX M3

or this:

41 PLANE SPATIAL SPA+0 SPB-37.3774 SPC+72 TURN FMAX SEQ- TABLE ROT

42 L X+2.7932 Y+3.0556 R0 FMAX M3

43 L Z+102.9597 FMAX

as the first point

And the cutting level coordinate is:

L Z+6.6055 FMAX

__L Z5.6055 F1000__

---------------------------------------------

#♫ PB, 5ax, itnc, nx, vericut ♫ #

#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: A CSE question?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-29-2018 09:45 PM

Dear Juraj,

Thank you very much.

I found the problem!

As you say "another thing machine simulation can overide postprocesor kinematics".

When I load the machine and the post result is (Wrong):

L X+44.5073 Y+2.0734 F5000.

L Z+88.392

L X+44.5073 Y+2.0734

L X+44.5079 Y+2.0734 Z-7.9621

L Z-8.9621 F1000.

L X+36.7579

When there is no machine and the post result is (Right):

L X+2.7925 Y+3.0556 F5000.

L Z+102.9597

L X+2.7925 Y+3.0556

L X+2.7931 Y+3.0556 Z+6.6056

L Z+5.6056 F1000.

L X-4.9569 Z+5.6055

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-30-2018 04:36 AM

you can put "return" in "pb cmd reload iks parameters" and you disable that overiding

---------------------------------------------

#♫ PB, 5ax, itnc, nx, vericut ♫ #

#♫ PB, 5ax, itnc, nx, vericut ♫ #

**Learning Advantage** Learn NX CAM online at your own pace (Login required)

**Manufacturing Tutorials**

Already have NX CAM installed? Get hands-on with the in-software tutorials

**Product Support**

Contact Global Technical Access Center (GTAC)

Follow Siemens PLM Software

© 2019 Siemens Product Lifecycle Management Software Inc