Auto length update based on sketch line? 1

[cygnas]

To make my question as simple as possible, assume I have a sketched line 24" long. Now, I have a steel rod extruded along that line that I would like to automatically update based on the length of this line. Example, I make the line 30" long and the steel rod is now 30" as well. It seems like a relationship could be used here somehow. What is the best way to do this.
TIA,
Drake

When it comes to protecting yourself or your family it is better to be judged by 12 than carried by 6.

 

[ctopher]

Make a 3DSketch and sweep along the line, is how I do it.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
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[CorBlimeyLimey]

You could use an Equation or, instead of a line, offset a plane & extrude Up to surface selecting the plane.


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[J-C]

"Up to Vertex" in the Extrude dialogue's "End Condition" and select the sketch lines endpoint.

Jason

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[CorBlimeyLimey]

Doh ... I always forget the easy one. "Up to vertex" is the way to go.

Star for you Jason.


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[cygnas]

ctopher, Is there a reason to use a 3DSketch rather than a 2D?

Drake

When it comes to protecting yourself or your family it is better to be judged by 12 than carried by 6.

 

[CorBlimeyLimey]

Just thought of another way ... use the Link Values feature, to link the dimension from the line length & the extruded length dimension of the steel rod.


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[CorBlimeyLimey]

cygnas ... just a passing thought, but you do know that you can access & change the length of the extruded steel rod, by double clicking it ... right?? You would have to do that to the sketched line anyway!


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[ctopher]

cygnas,
I use 3DSketch because I never know when/if it will change from a straight line to a curve. Editing the 3DSketch and rebuild, the sweep feature will change. If yours will always be a straight line, then the suggestions from the others above will work great.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[ashleygibson]

Why wouldnt you just drive the length of this by the features own dimension.

Having a sketch dimension drive the length of a feature is like holding a pen in your right hand, and using your left hand to move you right hand?

Unless you are using your sketch line as an undefined line and free moving its end into position then allowing it to build.

This is ok if each different length is a new part, but if not then each length will require it own config....and a dimension to drive the length, therefore why not use the feature dimesnion as mentioned above.

Design tables may be helpful here.

cheers

 

[bkelsey]

Have you tried the Weldments tools yet. It works pretty slick for extruding predifined cross sections along 2d and 3d sketches. There should be a tutorial for it too.