solid works help needed

I imported extrustion from into solidworks. Is there a way to elongate a part once it is extruded or do I have to mate all of the small parts together to get the length that I want. Thanks

To really answer this question I would need to actully know what your background and/or experience is in Solidworks, and what the part actually was…

But… to take a shot in the dark so to speak, I am guessing that you have a part you brought in and it came in at a fixed length and you would like to make it longer (or shorter - that will work too).

What you want to do is click on the end of the part, and start a new sketch on that plane.

Then you can use the “convert entities” button in SolidWorks (looks like a little cube with all black lines except for one red line - it is on the “sketch tools” toolbar in case you don’t have that showing) and select all the individual (or one large if that is the case) lines that make up the profile.
What that allows you to do is then, use that profile as your “new” sketch.
And then all you have to do is either make an cut-extrude to shorten it, or a boss-extrude to lengthen the part.

Hope this helps.

Or, on the original Extrude feature, you can right-click on it and choose Edit Definition – then change the extrude length to be whatever you need.

Be aware that, at least for the extrusion from that I’ve used, the sketch has no constraints built in and isn’t square. It’d be wise to go in and add constraints to that sketch first before you do anything further.

Yes, as M. Krass said, there may be problems with the lack of constraints when you make the new sketch or even work with the old one, so just keep putting constraints and dimensions until every line is black, Because as my professor kept telling us “Black is beautiful”

I was going to say that too, but most of the extrusions and parts I have brought into SolidWorks from have all been considered “imported parts” and not able to be easily edited. This is probably the reason for the original question… If it were just as simple as to modify the length of the original feature in a dialog box of some kind, I don’t think he would be asking what he is asking - but then again, you never know!

Whenever I’ve opened IGES-format files in Solidworks (2003), it’s automatically proceeded with feature recognition and made the part editable. It’s a part of Featureworks, which may or may not be included with Solidworks – I’m honestly not sure.

With IGES format I think it depends on how complex the part is.

Extrusion is a pretty simple part and very important- you would probably be happier redrawing it in SW (unless you enjoy fixing hundreds of broken mates : ) ). You can use the measure function to get dimensions and (as stated above) the convert entities to get profiles. What I would do is project the cross-section profile onto a new sketch using convert entities, copy that sketch, then paste it into a new part file and extrude it.