Unbend -- IGES Sheet metal

Hi Pro Gurus, I am having a sheet metal part as IGES format.I need to find out the development length of the part using Pro/sheetmetal or any other cad
packages. Any help in this regard will be greatly appreciated. Thanks in Advance.
Vijayarajan.M Member - Operations Pricol Technologies http://www.pricoltech.com
Pricol - Plant 1 Coimbatore - 641 020 India
Ph: ++91-422-2692901 Fax: ++91-422-2692028
E-mail: snipped-for-privacy@pricoltech.com
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: Hi Pro Gurus, : I am having a sheet metal part as IGES format.I need to find out the : development length of the part using Pro/sheetmetal or any other cad : packages.
In Wildfire, it's pretty simple. Create an empty part, import your iges data with 'Insert>Shared data>From file'. Select your iges file. Accept the defaults for placement. Go to 'Applications>Sheetmetal' and the sheetmetal conversion menu manager appears. Select 'Driving surf' and select one of the surfaces of your part. It should give you a thickness dimension which, if it is correct, accept it and it converts your part to sheetmetal. Then create your flat pattern by picking Feature>Create>Sheetmetal>Flat pattern. Use detailing to document the design or just use the Measure tool to get the dimensions. Also, using Modify and picking the flat pattern should show you all the developed lengths at the bends.
David Janes
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David, I have both step and iges formats of the part. After importing into Pro/E, I am unable to convert into sheet metal due to data loss. How to fix the problem? Is any import setup option is available in Pro/E? or any export setup option is available in UG or SW from which the IGES file is generated to compactable with Pro/E?
TIA,
Vijay.

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: David, : I have both step and iges formats of the part. : After importing into Pro/E, I am unable to convert into sheet metal : due to data loss.
Sorry, I forgot to mention this, but when the original part was exported as a solid, it wouldn't convert to a sheetmetal part in Pro/e. But, when it was exported as surfaces, it came into Pro/e and converted fine. If you have any of that kind of control over the export, try exporting it as iges surfaces.
Also, expecially on sheetmetal parts, with their very high ratio between part size and sheet thickness or small hole sizes, accuracy is a serious issue. Make sure any settings governing accuracy in the creating software are set high enough. A quick check of smallest feature to largest will tell how to set it. If that ratio is, say, 1:1000, set the accuracy to 1:1500, just to be on the safe side. Regenerate and re-export. This often fixes data integrity problems.
David Janes
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