Sheet metal flat pattern max dimensions

[Lars1978]

Hi All,

When i've made a flat pattern out of a sheet metal plate. I'd like to know the size of the flat pattern.

I'd like to have this as an part attribute.

What is the most easy way to produce this attribute?

Lars



Lars
NX12.0.2.9 native
Solid Edge ST10
Inventor

 

[Dave K]

You should be able to create a measure, of the surface area of the flat solid, and/or other dimensions for it. Create your attributes, and tie them to the expressions that the measure(s) create.

-Dave

NX 11, Teamcenter 11

 

[Lars1978]

Dave thnx.

Can I set this up in a template so I don't have to do this everey new part ?




Lars
NX12.0.2.9 native
Solid Edge ST10
Inventor

 

[Dave K]

Worth trying. Much like assigning some weight attributes, to pass on to the drawing, you'd probably need to create a sheet metal part, create the measures, then figure out a way for the measures to remain, once the sheetmetal part is gone...or leave the sheet metal features, and the user would have to edit them.

Definitely take some experimentation.

-Dave

NX 11, Teamcenter 11

 

[cowski]

I'm not sure how well this would work in a template, but perhaps you can create the flat solid then use the bounding body command to find the extents and use some associative measurements to find the overall size. Part attributes could be created that reference the measurements.

www.nxjournaling.com

 

[frankbe]

NX11 already has the max X and Y values for the Flat Pattern.
It won't be a part property though because NX allows you to create more than 1 flat pattern in a PRT file.

I hope this helps,
greetings,
Frank


2x NX11.0.2.7 Mach Design
on win7 64bit
NX Beta Tester

 

[Lars1978]

Frank,

That looks promissing. Where can I read this values outside the information window.

I'd like to put them into the part attributes

Lars

Lars
NX12.0.2.9 native
Solid Edge ST10
Inventor

 

[cowski]

They are saved as attributes on the flat pattern feature.

www.nxjournaling.com

 

[Lars1978]

Cowski,

I can't see the flat pattern attributes in the part properties....?

Can I solve this?

Lars

Lars
NX12.0.2.9 native
Solid Edge ST10
Inventor

 

[cowski]

You can create a part attribute that references the feature attribute; one strategy involves creating an intermediate expression to accomplish this. Assuming you have a flat pattern already created in your part:
[ul]
[li]Open the expression editor, create a number (length) expression with your choice of name[/li]
[li]for the formula, choose "reference object attribute", select the flat pattern feature from the part navigator, select the desired attribute and press OK[/li]
[li]An attribute expression will show up in the expression list (make sure the filter is set to "all" expressions). For me it was "p11 (Flat Pattern(5):Minimum X)". You can use OK or Apply to create your expression, though it isn't really necessary since we now have the correct system expression (p11, in my case).[/li]
[li]Create a part attribute that references an expression; reference the system attribute expression or the intermediate expression that you created.[/li]
[/ul]

www.nxjournaling.com

 

[Lars1978]

Cowski,

Is it possible to set this attribute thing up in the template. So when I make a new sheet metal part the flat pattern vallues are usable in the draft?
I don't like to set all attributes for each new (sheet metal) part.




Lars
NX12.0.2.9 native
Solid Edge ST10
Inventor

 

[cowski]

The flat pattern size attributes won't exist until you have a flat pattern. This will make it tricky, at best, to set it up in a template. One possibility may be to create a generic tab feature and flat pattern in your sheet metal model template. When you start a new part, you would resize the tab and add your flanges and other features as necessary; since the starting template has a flat pattern, you can reference the existing attributes and expressions. It used to be that you could only have a single flat pattern and it was always at the end of the feature tree; however, now that you can have multiple flat patterns timestamped throughout the feature history, I'm not sure how feasible this solution will be.

www.nxjournaling.com

 

[Lars1978]

hmz... making a journal can fix this ?

Lars
NX12.0.2.9 native
Solid Edge ST10
Inventor