I am new at pro/Engineer sheet metal. I made a U shaped beam, with holes and cuts on it. Now i need a symetrical part, have same holes and cuts on it but bended to other side. I mean that part will have same cut mold but will be bended to other side. I do not prefer using symetri feature, because i want to have 2 parts on different files but i want o have this files depended to first one so when i make changes other will regenerate automaticly.
Can i make this with unbend and bend back? or something like this? When i try this Pro/E always bending to same side again. I couldn bend to different side.
There are multiple ways to achieve this with Pro/E. Here's one technique:
You can create a new, opposite hand part model by assembling your original sheetmetal part to a new, Pro/E Assembly model and then using the functionality for creating a new component. This functionality allows you to make your new, opposite hand part model reference the original sheetmetal part, so that changes to the original model will propagate through to the opposite hand part model. Of course you can also just make it a stand-alone, opposite hand part model as well using the 'Copy' option instead of 'Reference'. If you don't want to maintain an Assembly model just to create an opposite hand part, follow the instructions below:
1) Create a new, EMPTY Assembly model. Make sure not to use your company's Assembly template model to start from. Just choose File, New, Assembly from the Pro/E menu structure.
2) Assemble your original sheetmetal model. You do NOT have to have an Assembly datum coordinate system feature or datum planes to assemble your component. Just use the icon for placing the component at the default location.
3) Use the functionality for creating a new component in Assembly mode--with the radio button labeled 'Mirror'. You will be given the opportunity to enter a user-defined filename for your mirrored component.
4) Reference the appropriate default datum plane to mirror your component about. NOTE: It absolutely does not matter if your resulting mirror copied part model geometry ends up inside the geometry boundaries of the original part model. You will end up throwing away the Assembly model anyway in the next step.
5) After you have successfully created your new, mirror-copied(opposite hand) part model, choose File-Erase and clear the temporary/throwaway Assembly model from session.
6) Choose File-Open from In Session and retrieve the resulting mirror-copied part model and File-Save it.
By utilizing this particular methodology, you won't have the baggage of maintaining an unwanted Assembly model. NOTE: If you do use the 'Reference' option for creating your mirror-copied part model, you'll always bring the original part model into your session(RAM/memory) of Pro/E whenever you retrieve the mirror-copied, opposite hand part model. Changes to the original part model will propagate through to the mirror-copied part model, but feature additions to the mirror-copied part model will not affect the original part model. Unless I am mistaken, the mirror-copied part model will have a feature in it named 'Merge'. I haven't had a need to do this yet in WF1 or WF2, but it was that way in prior release of Pro/E.
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