Unable to create a Flat Pattern from Derived Sheet Metal Part

[JimStrenk]

The company I work for has a large number of Left Hand and Right Hand sheet metal parts. To reduce the amount of time needed to create both Left Hand and Right Hand sheet metal parts, I use the Derived Part icon.  I create a Left Hand part, use the derive icon with mirroring on and create the Right Hand part.  While the Right Hand sheet metal part gets created, the Right Hand part will not allow me to create a Flat Pattern.

what steps must I follow to create a derived sheet metal part that I can make a Flat Pattern with?

[stevec781]

I do something similar except I create the mirrored part by mirroring in the assembly.  I find the sheet metal properties dont get copied corretcly so I have to go in and edit the sheet metal defaults.  After that it flattens fine.

[JimStrenk]

Thanks Steve for the reply.

Could you flesh out the procedural steps using a mirrored assembly as you've suggested?

[JDMather · Accepted solution]

The most common problem is forgetting to set the sheet metal style thickness in the Derived Component.

Attach file here that exhibits this behavior.

[stevec781]

In the assembly containing the sheet metal part just select mirror on the component tab, then once thats done, open the mirrored part and update the sheet metal settings and create the flat pattern.

[JimStrenk]

Forgetting to set the derived sheet metal part's thickness equal to the orriginal part's thickness was the key.  They must match for a derived part to be created.

Looking through the help files and all, I didn't see anything about the workflow need to derive a sheet metal part.  Could you or someone else provide us with the correct workflow (icon usage and settings) to correctly create a derived sheet metal part that behaves exactly like its parent?

Thank you for your asssistance J.D., it is appreciated!

[freesbee]

Thanks to these hints I could get a derived component that I can unfold.

To my needs, it would be better to be able to derive directly the flat pattern, and use it as my derived component in a new assembly (component origins and planes would be much better handled).

Reading around I have found that it should be possible, selecting the "Flat Model" with the "object selection tool" of the derived part command. I tried several times to select the flat model of my base component, but the derived part remains bended.

Does anyone know how to directly "derive the flat pattern" of a sheet metal part?

[will_hebden]

Ok, so i understand that you have to update the sheet metal styles (on the mirrered component) to match that of the orriginal part, but.... when i create a mirrored sheet metal part, all sheet metal rules dissapear, apart from  the default rule (see attachment). Does this mean that i have to import the correct sheet metal rule / unfold into the styles editor before i can do this??

This seems like a long winded work around for something that, after reading many posts on the subject, appears to be a pretty common problem? why don't the sheet metal rules copy across?

Note: this happens if i mirror the part through both the derive comand within the part environment, and also through the mirror comand from within the assy environment

[will_hebden]

Sorry, I stand corrected, this only happens when mirroring a component from within an assembly, not from mirroring using the derive comand from within the sheet metal part environment.

Is this issue (mirror sheet metal parts from within an assembly) resolved with the latest release? (2013)

Regards Will

[freesbee]

thi is the trick:

1. make a new sheet metal component

2. derive the original (say LEFT) sheet metal component making the mirrored version (RIGHT), and derive also the sheet metal parameters that you need (at least the thickness)

3. create a new LOCAL sheet metal style, calling it (for example) "Adaptive"

4. in the "thickness" field of this sheet metal style, write the value of the parameter coming from the other part (if parameters have the same names in the two files it will be something like "thickness_1"). Be aware that you cannot do it from the parameters table: you must do it from the sheet metal style editor.

5. make the "Adaptive" sheet metal style active.

Now your "RIGHT" part will unfold correctly.

How many sheet metal parameters you need to derive depends on how good you have based the Adaptive style on the actual thickness parameter. If you have done a good job you do not need to derive other parameters

[lilia_fellini]

There are two important step as I see to enable flat pattern in a mirrored/derived sheet metal part:

1) If starting with a new part, make sure you create a sheet metal blank part, not a solid

2) Set Sheet Metal Defaults if they failed to set up correctly during the deriving process

3) If still no luck - delete the flat pattern and generate it again after making sure points 1&2 are in place.

Hope it helps.

[dkd_in]

Hello, I face a typical problem while mirroring sheet metal parts. I explain the scenario here. Sheet metal Conveyor has LH and RM chassis parts. Everything is OK as far as mirroring is concerned, until there is text engraving / Template name. If I want text engraved/cut on to chassis I am in trouble as it also gets mirrored. If I want part to be mirrored but not the text, is there is easy way out other than putting text separately in dwg file before laser or plasma cutting process. I have attached reference image for ready reference, in which I have put text in assembly and used mirrored ipt parts. Now the challenge for me is how to generate dwg files for laser cutting operation.

[freesbee]

Hi dkd_in!

Whenever I had to punch left and right sides of sheet metal parts differently (as it happens with a logo, but also with a "conveyor belt shuolders with engine on one side and bearing support on the other side") I always used the following trick:

1. model the "MAIN" component with all common punches (i.e. holes for transversal beams present on both parts). This component is only a "logical component" and will not be mounted in the assembly. Model it left or right depending on your specific needs

2. derive* the "LEFT" part mirroring on the suitable plane, and punch the "LEFT specific" features

3. derive* the "RIGHT" part WITHOUT mirroring, and punch the "RIGHT specific" features

4. mount the 2 derived components in your real assembly.

That's it!!

* read the rest of the post to understand how to derive properly sheet metal parts that can unfold

BUT

this is a wonderful trick for engine/bearing supports or similar stuff.

Unless you don't have special rendering needs that force you to have the logo punched in the 3D model, I would personally nest the LOGO afterwards on the DXF.

Enjoy!!

[Mario428]

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@dkd_in wrote:
Hello, I face a typical problem while mirroring sheet metal parts. I explain the scenario here. Sheet metal Conveyor has LH and RM chassis parts. Everything is OK as far as mirroring is concerned, until there is text engraving / Template name. If I want text engraved/cut on to chassis I am in trouble as it also gets mirrored. If I want part to be mirrored but not the text, is there is easy way out other than putting text separately in dwg file before laser or plasma cutting process. I have attached reference image for ready reference, in which I have put text in assembly and used mirrored ipt parts. Now the challenge for me is how to generate dwg files for laser cutting operation.

---

We do many conveyors as well and have the same challenges if the 2 sides are different.

But this is where adaptivity may actually work, do most of the work on one side and make the common features adaptive. Each side then gets its unique features.

Bent shape could even be done using an excel table.

Would not use a mirror part in this situation.

[stevenmcalear]

I did this and the flat pattern of the newly created part is exactly the same as the Folded version (it did not work). My sheet metal defaults of the new part were changed to be exactly the same as the original, and the original part has a flat pattern that works.

any idea what this could be?

[JDMather]

You have replied to an ancient thread.

Attach your file(s) here.

[ali.jahed]

You are the man....Thanks 🙂