I have a pipe I created using the Sweep commands. I need to supply the shop with the straight pipe length. How can I straighten to measure the length? Or find out OAL ?
I have a pipe I created using the Sweep commands. I need to supply the shop with the straight pipe length. How can I straighten to measure the length? Or find out OAL ?
Kenneth,
Take a look at this post here, a lot of great ideas that should give you the answer you're looking for.
I am a little confused when I looked at the post because they are using an step file.
I have lots of different sizes similar to the first one. I am looking for the quickest way to find out the OAL of the straight piece.
The guys on the post have so many steps to find what should be a quick answer?
Kenneth,
If you want a quick answer you can just edit the 3D sketch, select all the geometry of the Sweep path & SolidWorks should give you a combined length in the bar at bottom right. You could also use the Fit Spline command on your selection & get a combined single spline with a single length that is dimensional.
Welcome to the forum. Are you acquainted with the Structural Member function on the Weldments toolbar? If you are, re-create your pipe profile sketch in a separate Part file, save it as a library feature part (.sldlfp), and use the line that you used for your Sweep path to create the pipe as a weldment. Then the software will automatically generate the length as a cut list property. (Even if you aren't familiar with the function it might be worth looking into.)
Does it work to copy and past the sketch I already created?
Yes, this may be of help 2017 SOLIDWORKS Help - Weldments - Creating a Custom Profile
You should check to see if a standard weldment profile isn't readily suitable first.
As I'm thinking about this, you should also be able to edit your path sketch, adding a driven Path length dimension to the series of lines (see the simplified example below). It's then possible to link this dimension to a custom property in the Part, and then link a Note or BOM column in the drawing to the property. You could of course just copy this value and paste it into your Drawing, but by linking them any later model changes will be reflected in the Drawing without additional user input.
Edit: Never mind. I don't use 3d sketches much, and wasn't aware that the Path Dimension function isn't available in them. Thanks to John Burrill for straightening me out on that.
Unfortunately, you can't create path in a 3D sketch. If you could, this would be pretty simple. Add the sketch entities to the path. Add a path length dimension, set to the value you want.
create a straightened pipe with the length dimension set equal to the path length. If the pipe layout is 2D, you can go this route
As it is, you'll need to set up an equation that adds up the lengths of each segment of the sketch. you can dimension arc and spline lengths. You just need to do a trick with your selection when you create the dimensions.
Once you've dimensioned the sketch segments of your path, you can create an equation relating the length of a straight pipe sketch to the sum of the lengths of the bent pipe segments (see attached)
I think, if you use the routing module to do the pipe system layout (you can use metal tubing or conduit) then you can insert a schedule summary into your drawing that will show you your unbent length. You might want to look into that because it can also account for material stretch/shrinkage during bending operations.
Good luck.
You have to Ctrl or Shift select the geometry to get the Total Length to show. If you draw a box around the geometry or right click & Select Chain the Total Length doesn't show for some reason.
..after using "select chain" just LMB on one entity then you will get Total lenght. This should also work with "filter sketch segments" and select all (CTRL-A).
Thanks Krzysztof,
That's good to know. Works great on Select Chain & Filter Sketch Segments but not with Ctrl A as it picks dimensions for fillets or lines & also intersection points of lines before fillets. Of course Ctrl A will work if you stil have Filter Sketch Segments on.
Exactly. That's what I meant.
I'm not very good at writing in english and sometimes my answers are a little bit chaotic
Those of you that have to unbend tubing a lot, I recommend looking into Tube Works software. We do a lot of bent tubing here and Tube Works is a great time saver. It is an Addin to Solidworks. It creates the 3D sketch, flattens the tube if so desired and creates a table with the XYZ coordinates for tube bending equipment. I love it.
Just right click the sweep sketch and select tangency and then the measure tool. It will give you the total length.
Steve C
Steve
what do you mean by select tangency
I meant to say select chain. In my posting above, if you right click the path of the sweep and select the chain, you'll get the entire path.
Steve C
Thanks every one for your help. Lots of great ideas.
I used Steve Calvert's idea to measure the OAL with measure. Then I made a flat configuration of the part to show in a 2D in the drawing. Only thing I am concerned about is the two configurations do not update with each other. I will have to try and figure out a equation that adds up the lengths. Keep getting errors with my equations.
Thanks to all
Ken
We have 2 tube benders here so we just output coordinates for the machine.
If you liked my response and it solved your problem, please mark it as the answer.
Steve C
Please try my superMacro and let me know if it works for you.
We have 2 tube benders here so we just output coordinates for the machine.
If you liked my response and it solved your problem, please mark it as the answer.
Steve C