Sheet metal flat pattern problems

[SiW979]

The majority of our products are based on large weldments that we use NX sheetmetal to design and create the flat patterns. Sheet metal to us can be up to 25mm thick, and in many cases we need to add chamfers to edges which are basically weld preps. We have recently started seeing issues cropping up where the flat pattern is not forming properly, as per the attached model. This means that we can no longer create the flat pattern in the model file because the flat pattern will always jump to the last feature, instead, we are returning to an old method we used to use where we WAVE linked the part at a time stamp before the chamfers were created in the Master Model drawing and creating the flat pattern from the wave linked body. It works, but its a bit of a pain in the rear doing all these extra steps. Should NX be able to handle features like these considering that chamfer is presented as a feature on the sheet metal toolbar?

Best regards

Simon NX7.5.3 - TC 8

http://www.jcb.com

 

[jerry1423]

Only within the last week have we moved up to NX7.5, and the flat pattern issue that you are experienceing is one heck of a bummer.
I can only off a work-around: extract a body after the flat pattern feature and add the chamfer to that, obviously you now have the issues of dealing with two bodies.
I am glad to see this brought up here, so I know what is in store for me. I wonder why that did this ?

 

[SiW979]

Jerry

It's a real disapointment, as we were really impressed with the new flat pattern button and how robust it seemed during testing. We thought of the extracted body option, but hassle of sorting out reference sets and layers means for the time being we will jsut carry on as we have detailed in our CAD standards of WAVE linking in the drawing at time stamp to omit the post cutting machine ops then suppress the WL body once we have taken the flat pattern from it. I looged an ER today because the best thing I could see as a way to fix this is to allow the user to specify a time stamp for the flat pattern in the model so the chamfers are not taken into account as currently the flat pattern can only ever be the last feature in the tree. Also we have instances were a chamfer just doesnt cut it and we have to created weld preps using sweep along guide etc and again these aren't handled at all well by the flat pattern tool.

Best regards

Simon NX7.5.3 - TC 8

http://www.jcb.com

 

[jerry1423]

In the customer defaults "Sheet Metal (forming & flattening)"
There is a toggle under the "General" tab that reads "Enforce Creation State Editing"
The default is "unchecked", so it may be worth it for you to check it "on" that
and see how that affects the model.
I couldn't find anything in the doc about it.

 

[JohnRBaker]

No, I don't think that will help. If while in Customer Defaults, you were to hold your cursor over the small '?' next to the option, a short description of what this option controls will be displayed and I think, when you read it, that you see that it's not relevant to this situation.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[jerry1423]

That's funny - I put my cursor over the question mark and nothing comes up.

 

[JohnRBaker]

It's always worked for me:

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[frankbe]

Do you have NX8? I believe it works there without any problems. The flat pattern shows a dash lined curve representing how far the chamfer should go.

2x NX8.0.0.25 Mach Design
1x Solid Edge ST2

 

[JohnRBaker]

I tested this using NX 8.0 (actually NX 8.0.1.5) and while the behavior has not changed in the sense that the 'Flat Pattern' is still the LAST feature in the tree, at least there is no longer an 'update' error when editing the Chamfer.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[SiW979]

Either way, I think giving the user the choice as to where the flat pattern is created in the model history would allow the use of other modelling operations that are currently causing needless problems.

Best regards

Simon NX7.5.3 - TC 8

http://www.jcb.com

 

[frankbe]

Hi Simon,

I will most probably attend beta testing sheet metal for the next NX release and I will put this on my agenda. Allthough I hardly ever run into situations like that myself, I can see great added value in what you're asking.

I'm just thinking of sheet metal parts that need machining after being bent. With the solution that you're proposing this kind of work could become very easy to deal with.

NX already allows multiple flat patterns to be created of the same part. It would be very meaningful to have the user option to make a specific flat pattern stick at a specific point in the history tree.

2x NX8.0.0.25 Mach Design
1x Solid Edge ST2

 

[SiW979]

Frank

I'm involved with the Beta testing in the UK too, so I'll be bringing this up as well, but the more the merrier!

Best regards

Simon NX7.5.3 - TC 8

http://www.jcb.com

 

[jerry1423]

What I would like to see in NX is the ability to force (as an option) a feature to be the last one in the tree.
It couuld be a flat pattern (like this), or a body measurement feature, or a solid that is related to the inside volume of a tank, or something else.

 

[cowski]

And if you mark multiple features to be the last one, what should happen?