Cancel
Showing results for 
Search instead for 
Did you mean: 
Highlighted

"Analyse Formability-One step" cuve extruded and unite with main sheet metal will creat extra body

Experimenter
Experimenter

I am trying to unfold the dimple feature on the sheet metal and creat intemediate stage for die design,I got the anylisized curve from one step analyse, then extruded , after cutting the extra body, I trying to unit the main sheet metal body with the new extruded area,but it reminds the following information and exacted body will be created, the orignal body and exacted body are seperate,they were not united,when I use old version of NX 8.5,it seems there was no such problolem,but the new version NX12 got this problem, would be apprecaite if someone could point me in the righ direction,thanks

20171204110642.png

10 REPLIES

Re: "Analyse Formability-One step" cuve extruded and unite with main sheet metal will crea

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @davidkwock

Try this alternate solution:

- Change to sheet metal application

- Convert the body to sheet metal

- Create the one step feature with parameters of your choice

- Remove the Dimple portion using Normal Cutout (select dimple curves (not one step Spline)

- Add Secondary Tab feature and select outer one step curves (use Connected curves with stop at intersection for selection tools)

- Create flat pattern

 

I have attached my version and shown the steps in the moview below

(view in My Videos)

 

Dave

Re: "Analyse Formability-One step" cuve extruded and unite with main sheet metal will crea

Creator
Creator

Hi,

 

My observations, questions and thoughts:

I made a simple tab + dimple, did the 1step formability analysis and added an Extrude (with Subtract) - all in Sheet Metal application in NX 8.5, 11 and 12.

In NX 11.0.2 it's still as usual, in NX 12.0.0 there is that change with the automatic extracted body. I don't understand why this automism? Maybe there is a sophisticated explanation and it's meant good. But for me (and I'm afraid for the most users) it's overcomplicating the thing. When I need an extracted body then I can do it on my own.

Yes - when I do an SB Normal Cutout instead of Extrude+Subtract, then I don't get a the extracted body. But in the end that's a little bit inconsequent...

Seriously: Why the automated creation of the body? We didn't need it in the past. Now we need workarounds to avoid it, respectivly we have additional work. What is the improvement?

 

Best Regards,

Thomas

Re: "Analyse Formability-One step" cuve extruded and unite with main sheet metal will crea

Siemens Phenom Siemens Phenom
Siemens Phenom

@bshkoerner wrote:

Seriously: Why the automated creation of the body? We didn't need it in the past. Now we need workarounds to avoid it, respectivly we have additional work. What is the improvement?

 


I'll have to ask the modeling/surfacing team about this one.

Dave

Re: "Analyse Formability-One step" cuve extruded and unite with main sheet metal will crea

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi all,

Here's the answer...

 

There is a new modeling preference: 'Treat Degree 1 Spline as Polyline'

Turn that off and everything works as before.  This is set to ON to support Convergent Modeling where this geometry is most prevelant.  It was mentioned in the 'NX11 What's new' for convergent modeling however it appears that no real detail has been added to the help documentation; that is still work in progress.

TreatDegree1SplineasPolyline.png

Re: "Analyse Formability-One step" cuve extruded and unite with main sheet metal will crea

Experimenter
Experimenter

Dave, thanks for your help, it seems this method is not working by unchecking degree 1 spline as polyline, can you double confirm?

Re: "Analyse Formability-One step" cuve extruded and unite with main sheet metal will crea

Siemens Phenom Siemens Phenom
Siemens Phenom

@davidkwock wrote:

Dave, thanks for your help, it seems this method is not working by unchecking degree 1 spline as polyline, can you double confirm?


I tried this with the option unchecked and did not get the alert about facet body.

Can you confirm the workflow steps you are doing?

My method:

- Convert to Sheet Metal

- One Step (Element size = 1.3). Select as per movie posted earlier.

- Extrude (selection intent = connected curves). select one step curves + dimple tangent

 

I do note that this method leaves some parts not cut away - is your method different?

2017-12-05 07_47_55-NX 12 - Sheet Metal.jpg2017-12-05 07_50_04-Clipboard.jpg

Re: "Analyse Formability-One step" cuve extruded and unite with main sheet metal will crea

Creator
Creator

example.pngMy Exampledeg1_on.pngDegree 1 Spline as Polyline: ON

deg1_off.pngDegree 1 Spline as Polyline: OFF

On my installation/example it works as Dave described it. After some thinking, I believe it even could make some sense :-)

But the information politics ...

Re: "Analyse Formability-One step" cuve extruded and unite with main sheet metal will crea

Experimenter
Experimenter

Thanks, Davy, after re-try the problem have been solved, but I have to uncheck this box every time restart the software.

Re: "Analyse Formability-One step" cuve extruded and unite with main sheet metal will crea

Siemens Phenom Siemens Phenom
Siemens Phenom

@davidkwock wrote:

Thanks, Davy, after re-try the problem have been solved, but I have to uncheck this box every time restart the software.


It is a preference so the setting is saved with the prt file, you will need to update your template parts with this setting.

Dave

Highlighted

"Analyse Formability-One step" cuve extruded and unite with main sheet metal will creat extra body

Experimenter
Experimenter

I am trying to unfold the dimple feature on the sheet metal and creat intemediate stage for die design,I got the anylisized curve from one step analyse, then extruded , after cutting the extra body, I trying to unit the main sheet metal body with the new extruded area,but it reminds the following information and exacted body will be created, the orignal body and exacted body are seperate,they were not united,when I use old version of NX 8.5,it seems there was no such problolem,but the new version NX12 got this problem, would be apprecaite if someone could point me in the righ direction,thanks

20171204110642.png

NX Sheet Metal
NX Sheet Metal

This group is dedicated to the discussion of Sheet Metal in NX.

Members (79)