cancel
Showing results for 
Search instead for 
Did you mean: 

Output of RADIAL_GROOVE_MILLING

Valued Contributor
Valued Contributor

Hello!

 

It's about the operation RADIAL_GROOVE_MILLING. In the internal toolpath there are circular paths displayed in NXCAM. In the standard PPs (e.g. sim07_mill_5ax_tnc_mm or sim07_mill_5ax_sinumerik_mm) linear movements are written to the NC file. The same thing happens in our Heidenhain PPs. Only our S840D-PPs actually give out circular movements.Why do I get linear motions? Is that a special type of circular movement? "Normal" circular motions are written as circular motion. I can not understand it.

 

I'm very curious.

 

Werner

9 REPLIES

Re: Output of RADIAL_GROOVE_MILLING

Esteemed Contributor
Esteemed Contributor

I know (at one point) the default mode for Siemens 840D posts was to output linear moves even if there were arcs in the internal toolpath.

Given enough putzing with the post & UDEs, you could get arcs (and a warning about those settings).

But if you get arcs sith other operations in the same part, that may not be it

 

1) Try a fanuc control post (just create a generic post with appropriate 3/4/5 axis setup), and post your op, see if that gets arc or linear output

2) Check the motion output in the operation, make sure arc output on (I think this is already set, but just make sure)

3) See if using the ENV variable UGII_CAM_POST_ENABLE_RESOLUTION_ROUND makes it better.

 

Ken

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Output of RADIAL_GROOVE_MILLING

Valued Contributor
Valued Contributor

Hello,

 

  • No, your standard fanuc control (sim07_mill_5ax_fanuc_mm also creates linear moves.

 

  • Yes, there are circular movements:

 

FEDRAT/MMPM,203.6000
GOTO/153.3600,61.5200,72.0000
CIRCLE/150.0000,62.5000,72.0000,0.0000000,0.0000000,-1.0000000,3.5000,0.0600,0.5000,50.0000,0.0000
GOTO/150.0000,66.0000,72.0000
PAINT/COLOR,31
CIRCLE/150.0000,50.0000,72.0000,0.0000000,0.0000000,-1.0000000,16.0000,0.0600,0.5000,50.0000,0.0000
GOTO/134.0000,50.0000,72.0000
CIRCLE/150.0000,50.0000,72.0000,0.0000000,0.0000000,-1.0000000,16.0000,0.0600,0.5000,50.0000,0.0000
GOTO/150.0000,34.0000,72.0000
CIRCLE/150.0000,50.0000,72.0000,0.0000000,0.0000000,-1.0000000,16.0000,0.0600,0.5000,50.0000,0.0000
GOTO/166.0000,50.0000,72.0000
CIRCLE/150.0000,50.0000,72.0000,0.0000000,0.0000000,-1.0000000,16.0000,0.0600,0.5000,50.0000,0.0000
GOTO/150.0000,66.0000,72.0000
PAINT/COLOR,37

 

  • What should I do with the environment UGII_CAM_POST_ENABLE_RESOLUTION_ROUND?
    Do I have to make it global in the post and then set to 0 or 1? What is your idea?

 

Werner

 

Re: Output of RADIAL_GROOVE_MILLING

Phenom
Phenom

I wonder if the kinematic settings in NX think your tool axis is slighly out of line. This will cause linear output. I lie to NX with my posts (set to table/table) for this reason. The cl post will not care about kinematic settings (it has none.)

NX10.03
Windows 7 Pro

Re: Output of RADIAL_GROOVE_MILLING

Esteemed Contributor
Esteemed Contributor

RE: UGII_CAM_POST_ENABLE_RESOLUTION_ROUND

The easiest way to test:

- close NX (save parts, etc. as desired)

- if in Teamcenter, close TC

- Right-click on “My computer” -> Properties -> (in column at left) “Advanced system settings” -> “Environment variables” button -> top half of dialog

- click on "New"

- set name to UGII_CAM_POST_ENABLE_RESOLUTION_ROUND

- set the value to "1" (without the quotes)

- OK out

- if in TC, start TC

- start NX

- post, see if you get arc output

 

If you find it works, undo-the above

Add to an ENV file, line like:

UGII_CAM_POST_ENABLE_RESOLUTION_ROUND=1

 

Ken

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Output of RADIAL_GROOVE_MILLING

The motions are "normal" circle motions, as you can see when you list the path or turn on the review tool.

 

I just tried the out of the box Sinumerik and Heidenhan posts in sim07, and got circle output, so I don't know what is different on your system.

Mark Rief
Retired Siemens

Re: Output of RADIAL_GROOVE_MILLING

Phenom
Phenom

Just be aware that kin variables "mom_kin_arc_output_mode" and "mom_kin_arc_valid_plane" and "mom_kin_machine_type" affect arc vs linear output (and there is a variable for max and min arc size.) It could be that the various posts could have differences with these.

NX10.03
Windows 7 Pro

Re: Output of RADIAL_GROOVE_MILLING

Valued Contributor
Valued Contributor

Hello everybody!

 

After comment from Mark I examined whether I've really tested with the newest OOTP-Posts. Wonder, wonder: NO!
In the newest OOTB-Posts there is a query about the mom_operation_type and the string "Radial Groove Milling". After changing my Heidenahin-Post to the same query I got circular output.

 

This are the things I would like to be alerted from SPLM. e.g.:

 

To all Post-developers: There is a new mom_operation_type called "Radial Groove Milling". Pay attention that this type is taken into account in the queries in your existing PPs.

 

It would not be very difficult.

 

Thanks to all.

 

Werner

Re: Output of RADIAL_GROOVE_MILLING

Phenom
Phenom

It looks like that routine shows up in V9. We are not there yet. Also - my guess is that OTB code is not used by the largest companies with the most seats. One that I know of makes most of their TCL without ever opening postbuilder (open the TCL they have developed in an editor.) The code underneath when using postbuilder is ever evolving. This is not reliable enough for some. Thanks for the heads up (I use postbuilder - not so much of the OTB template code though.)

NX10.03
Windows 7 Pro

Re: Output of RADIAL_GROOVE_MILLING

Esteemed Contributor
Esteemed Contributor

This is getting somewhat off topic, but other new mom_operation_type values are being set for

Hole/boss milling

chamfer milling

groove milling

probably some of the other holemaking operation types.

 

I haven't had a chance to get into the code to see what the actual values are, however.

(I, too, need to update my posts & tcl code)

Above found while testing NX10.0.2

 

I realize it's a moving target, but it would be nice if Siemens could document ALL the possible values for this variable  (hint, hint, nudge, nudge...)

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Learn online





Solution Information