Flattening parts 1

[engstudent18]

Hi there,
i am working for a company that asked me to take modeled parts given to us by clients and give a flattened drawing for the shop. Opening these parts, it will not let me flattened them. When I open them as a sheet metal part and click on tools then flat pattern then flatten, it says to pick on a face to orient upwards but then it wont let me click on anything. I try to just use the "save as flat" but it comes up with an error saying it not all parts are flattened. I have looked online but haven't found anything helpful.
Can anyone advice me how to take these modeled parts and give a flat pattern I can dimension for the machine shop?
Thanks

 

[SvenBom]

Did they give you *.par files instead of *.psm files? Or maybe step or iges files instead of Solid Edge psm files?
If you want to use flat pattern, you need to have proper sheet metal files. So, if you have par files, that you want to flaten, here is the procedure:
1. open those files in Sheet Metal environment
2. use the transform to sheet metal. In Solid Edge ST5, this command is in the Application Menu
3. select a face for an inital sheet metal face
4. click OK and the par file is converted to sheet metal.

But of course, this will work only, if the par file is modeled correctly for the sheet metal environment. This means, that the thickness is the same allover the part, the outer radius is inner radius+thickness, the edges of what has to be flanges must be separated, etc. If the customer files are not correctly modeled, then you will have quite some work to fix them.

Hope this helps.
Regards.

 

[prsyam]

Also if the part is made in a forming die, forget about solid edge, you have to use Fastblank for getting almost correct blank. More complex the shape, less accurate the blank.

 

[engstudent18]

Hey thanks so much SvenBom,
I tried this and when i went to transform to sheet metal it told me to select face and would only let me select one. When I did it came up with the error " Input model contains non-sheet metal faces that must be removed before transforming". Ever run into this error?
Thanks

 

[SvenBom]

Such error occur on cases, that I have mentioned before. I guess, that there is different thcikness on the model. Most of the errors in modeling, that I have seen were like this:
1. thicknes=1mm
2. inner radius=1mm
3. outer radius=1mm. This is te most common mistake, the not very careful cad engineers will do. In this case, outer diameter should be 2mm.
Then there is a problem with edges, that are connected. Imagein something like this:
1. create an extrude from a rectangle
2. apply thin wall or shell
3. now try to convert this into sheet metal. It will not happen. You have to first use RipCorner command and rip those connected edges.

And then there is the biggest problem:
1. the model is created with some surfacing like bluesurf, etc.
2. or the model has three or more round, that come into the same vertex. After saving such model into step or iges format, the transition between those round will most likely be converted into b-surface.
3. in those cases, I don't thinnk you will be able to convert the model into sheet metal. You will have to remodel everything in sheet metal application so, that it will be proper model for flatening.

I hope that this helps.
Maybe you can upload an image of the model or model itself, if you are allowed to do this, of course.

 

[SvenBom]

Here is also my video about using the Transform to SheetMetal and Rip Corner commands. The viedo quality is not to good, but you will get the basic idea of what is possible to do with those commands.

http://www.youtube.com/watch?feature=player_embedded&v=feh-NGFZtyM

There are some differences in nameing of the commands and their position (transform to SM or convert to SM, etc.). But the procedure is the same. You can see, that RipCorner works both on corners and on sketch lines.

Hope, this helps.
REgards.

 

[Kenny_G]

Excellent video SvenBom. Are you still working with ST (v100)?

Ken G.

http://grundey.blogspot.com

Have you checked out the Solid Edge Community site?

http://community.plm.automation.siemens.com/t5/Solid-Edge/ct-p/solid-edge

 

[SvenBom]

no, i am not working with st1 anymore. the movie is just one of my old ones. I am working with st5 now. And I am just waiting for my copy of st6. There are some excellent new features and options in sheet metal, drafting, etc.