Ok, so I have an STEP file with an assembly with different parts in it, but not the original part files. i want to change the dimensions of one of the parts. Is it possible? if so how?
If all you're wanting to do is make the cylindrical section of the part longer, here's how I'd do it:
1. Make a rectangular cut in the middle of the cylinder to cut the part into two bodies.
2. Use 'move/copy bodies' to move one of the new halves a distance along the parts axis.
3. Extrude the cylinder profile to join the two halves.
You might be able to do it with "FeatureWorks" I don't remember which version of SolidWorks you need for it. But it works for me
If you play with the feature and a step file for two minutes you'll know how to use it, its really easy.
You can turn it on (if you got it) by Tools->Add-ins. I hope you got it.
ps. you are not editing your step file you are replacing it with a SolidWorks files which you then can change! (If I'm not mistaken)
I just tried it, and I remembered that you have to place the dimensions that you want to change, in some cases its still faster than created the model from scratch.
I have seen one demo of SW2010 where they showed how one can easily edit the imported bodies. If you have SW2010, you can try out. Else depending on your part, you can create new features (i.e. add/remove material)
Deepak - You're correct. In 2010 you can RMB on an imported part's feature(s) and, if SW recognises that feature, makes it editable. This requires Featureworks to be available. Amir - have a look at this video for the demo Deepak mentioned http://www.youtube.com/watch?v=CSHRqNBNtSE
Yes if it has been run through FeatureWorks. We do this daily. As long as the Features are picked up by SolidWorks they are editable.
You can also just use the "move face" command, to alter the position of any face. Because there is no defined dimension, it is all relative. So "move face" 10 mm will add 10 mm to the dimension.
Thanks Charles,i have solidworks 2009 and don't seem to have featureworks, but your move face suggestion works. the only problem is that i want to elongate a hollow tube, whose top and bottom were filleted and attached to extruded circles. when i click on the "body" (round part) of the tube, and click "Move Face" and offset, solidworks wants to make the tube thicker, how do i get it to make it longer?
Amir - One way would be to split the part into two bodies then move one of the bodies by the amount you want to lengthen the tube. Then make an extruded feature on one of the bodies to join the two bodies back together (i.e. to fill the gap you just created by doing the split & move). Or do a move face on one of the newly-made tube faces.
thanks Keith, but can you elaborate a bit more? How can i split the tube and how do i stick it back together?
Move face should work, but I'll elaborate on the split/move/join technique...
Start a sketch on the plane that is parallel to the hollow tube.
Sketch a single line that crosses the tube (perpendicular to the axis of the tube), it dosen't need constrained or closed...just a line.
Select insert> feature> split, you should see the current sketch selected in the "trim tools" box, click "cut part"
This should leave you with 2 "bodies", one on each side of the "split".
Select insert> feature> move/copy, and select one of the 2 bodies you just split, then type in the distance you want to extend the pipe into the appropriate cell.
Create an extrude feature on one of the tube faces you split previously, to fill in the gap between the bodies.
When using the Move Face command, instead of chosing "offset" you should be able to use "translate". Then, instead of grabbing the outside of the tube, grab the end of the tube, and select a distance for the offset.
I tried what you suggested, and the program does something strange: the "move face" is registered on the design tree, and when double clicked shows a dimension that reads 10mm (the amount i wanted to elongate by) starting from the center of the tube, but no elongation is visible, do you know what can be causing this?
I'm not sure I can trouble shoot that from afar. Can you upload the .sldprt file? Maybe a screen shot if you can't?
Ok, heres a screenshot, perhaps you can see what went wrong.
You can also use the "split part" feature to do the slicing as well and then follow it with the move / copy body tool
thanks guys, the split/move method worked great for me:).
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