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Saving a feature as a separate part

MadPickinSkills

New member
Hello,
I was wondering if its possible to save a feature on a part to a separate part file. For example, If I created a model of a keypad and wanted to save the keys as their own part file and then create an assembly with both parts? I seem to remember doing something like that a long time ago but I cant remember.
 
I never see a feature saved as part.
In SW you can copy features from one part to other.

I do not understand how you create a keypad model ?
The keypad has (in my mind) the keys as parts.

Maybe if you provide more informations I can help you better.

Good uck !
 
Mihail said:
I never see a feature saved as part.In SW you can copy features from one part to other.I do not understand how you create a keypad model ?The keypad has (in my mind) the keys as parts.Maybe if you provide more informations I can help you better.Good uck !

Hello,
Thank you for the reply. The keypad was only an example I used to try and explain what I was trying to do. Think of it like I created a hammer, but now I want the handle of the hammer to be a separate part.
I am able to copy a sketch from one part file to another part file and then re-create the solid model from it, but I was hoping I could just copy or save the entire feature to a different part file.
Thanks
 
As far as I know, this is not possible.
Like in the real life, you must make a hammer from two parts.

BUT !!!!

You can use each part in other assembly(s).
For that you can copy a part file in other assembly's folder and modify it as you need (that ensure that you do not modify the original part - and the original hammer) OR you can make configurations for the part and use each configuration in different assembly (or in the same assy).
In that case, if you modify a configuration only that assembly(s) that use this configuration will be modified.
Note that you can make as noumerous configurations as you wish.

In the first case you have "n" separate files for the same part (one for each assy). That dramaticaly increas the storage memory.
In the second case you have a single file for part (slighty bigger in size than the original).

I say "hammer" as an example
smiley1.gif


Good luck !



Edited by: Mihail
 
The closest thing I could find to your situation would be to make sure the feature does not merge with your existing features. This will create a multiple body part. One of the context menu options for the body is to insert it into a seperate part. Then that body is it's own part that can be inserted into other assemblies. So in your keypad scenario you would model your base. Then when you started modeling the keys, e.g. extruding a rectangle for a simple key, you would uncheck the merge result box. You would then have a section in your feature tree called Solid Bodies. Right click on the body you want and click insert into new part. The feature manager in the new part will show a feature that is a link to the original part. Now you can make changes, insert in assemblies, etc. and it will not affect the original. I did not try it but after that you may be able to break the external reference link and use feature recognition to get a feature tree if it is not too complicated. Hope this helps you find a path towards your goal.
 
Thanks for the help all. I've been copying the sketch of the feature I want as a separate part and pasting it into a new part file. The down side is that I have to re-create it from there.
I will try the ideas you guys gave me.

Thanks again
 
Make the handle a separate body. Go to the first handle feature and uncheck merge parts. If the feature does not come out right, shift it up and down the menu until it has all the proper features that make it up. Then go to bodies at the top of the menu and select the handle body and import into new part.

I do this all the time when I want an assembly of dependent parts.
 
Try insert->features-> save bodies

Hello,
I was wondering if its possible to save a feature on a part to a separate part file. For example, If I created a model of a keypad and wanted to save the keys as their own part file and then create an assembly with both parts? I seem to remember doing something like that a long time ago but I cant remember.

Try insert->features-> save bodies
 
Hello,
I was wondering if its possible to save a feature on a part to a separate part file. For example, If I created a model of a keypad and wanted to save the keys as their own part file and then create an assembly with both parts? I seem to remember doing something like that a long time ago but I cant remember.

zzzzzzzzzzzzzzzzzzzzzzzzz
 
Last edited:
Would be cool if the SW developers would let you bring in the SolidBodies you exported. That would be almost like a copy Paste Special command like we have in Creo that I have grown to utilize so much in my design workflow.
 

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