I have some swept tube, and I want to calculate straight/cut length.
Is there any option in SOLIDWORKS?
you can take below e.g for ref.
Just measure the sweep path length and that would be length of straight pipe.
But I need to show it in drawing as a straight length.
Create two configurations; one straight and one bend. You can set up the length line equal to total lines in the bend sweep path. And then you can show both in the drawing.
You can create and equation for total length and then set the straight length equal to that OR simply create direct equation and add all lengths.
If this is something you'll be doing fairly often I'd recommend saving pipe profiles as library feature parts and using the Structural Member function on the weldments toolbar to create the bent pipe. If you do this then the length will be automatically calculated as a cut list property which can be called out in a note or table in the drawing.
Put a fit spline on your path (selecting all the lines) and dimension the spline.
Thanks to Deepak and all
Assuming your sweep path is the centerline of the pipe:
1) Create a path length dimension by selecting the entities of your path (in the path sketch). This creates a driven dimension.
2) Create a global variable and reference to this dimension.
3) Create a custom property and reference it to the global variable.
4) On your drawing, create centerlines along your path.
5) Create a leadered note to this centerline: add some explanation text and then link in the custom property from the part. Add parentheses since this is a reference dimension.
See the attached files.
I do this alot and like your method you described above. I tried this procedure on a simple pipe sketch in front plane only and it works nicely. Question though, I do not see an option to "make path" on a 3dsketch using straight lines and fillets in the x,y,z planes. Not really any need for this for what I do, but I'm curious how its done. Please see my sketches below. First is for the 2d sketch and second is for the 3d sketch which I'd like to use "make path" from so I could ultimately get the length I need to cut. Just wondering about the approach to be used. I only used 3dsketch lines and fillets, but I read online about needing to use splines and fit splines command possibly? Thanks in advance for any insight.
In your 3D sketch select one end of the sketch RMB and select chain then go to tools spline fit spline then you can dimension it.
I'm trying to RMB on an endpoint to 3dsketch but see no option for "chain". I'm on SW2015. I've attached file. Am I missing something? Thanks for your input!
Not the end point but the first or last line segment then RMB and select chain. Also once you have the fit spline close the sketch then use the dimension tool.
Thanks for the info Tony!
Try TubeWorks Add-In
You can flatten the tube to show in the drawing as well as adding elongation factor for when it is bent.
Create the section profile as a Square, insert Sheet Metal Bends, then you can flatten. You can add 4 corner radius's to make the final part round..
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