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I have been looking all over and can't seem to find a way of selecting a bend line in a drawing for dimensioning. In the part shown, I need to find the dimension from the left and top edges to the bend lines? I am using Solidworks 2022 Connected. Any help would be appreciated.
I seem to be late to this party, so if you're still waiting, here's at least an answer for you :)
The "technical reason" is that the "bend" line doesn't exist! It merely designates a "bend" while the part is being shown in the "flattened."
For this reason, you can't attach a dimension to it by using Smart Dimension or even with the DimXpert, nor can you assign any annotations through Right mouse Click and reading the in-context menu.
Let me give you two ways to do this, but then i'll explain why.
You can, of course, draw the part in the Flat, and then sketch in a "Bend" line. That function is available on the Sheet Metal Command Manager. OR, you can create your sheet metal part, flatten it, and then go to the Sketch Command Manager, enter into a Sketch after picking Plane or a planar face, then sketch in construction lines on top of the visible dash line simulating a bend location. You can smart dimension that line or lines, but leave the dimensions "driven" instead of "driving."
When you unflatten the part model, the sketch should be suppressed under the suppressed Flatten on the FeatureManager Design Tree. When You need to see it, unsuppress the sketch and left mouse click on "Show."
As to why all this is, I am assuming that the reason for this is because when someone brings in either a drawing or a file with the model, the sheet metal guys will normally figure out where and with what tools/dies to create the bends depending on your choice of material and what you're trying to accomplish. Hope this helps.
Not sure why selecting the edge and the bend line using the SmartDim tool won't work: Just tested it and it works fine for me.
Some setting set wrong? BTW, I projected the tangent lines and set them to center lines on the bottom bend, in my quick&dirty test.
Attachment 9161
http://eaaforums.org/image/png;base6...AAAElFTkSuQmCC
-Christian
Which version are you using just out of curiosity?
I have a 2021-2022 Student version where I can smart dimension tool the theoretical bend line in a drawing. I have a 2020 full version where I can't smart dimension the theoretical bend line unless I use the "sketch bend" feature on the Sheet Metal Command Manager, or I draw a sketch using construction geometry to accomplish it as described above. Also, did you customize that "dot-dash" line in your drawing?
(There are a lot of real cool features in 2022. It's been a few years since SolidWorks had this many cool features. Some years they pull out useful features just to increase the number of changes they claim they made. Removing the "Parent-Child" arrows in the 2016 version comes to mind. Those arrows saved time for me in 2014 and 2015.)
Floyd-
The triangle was created by a flat extrude, then add Bends (there were none), then add flanges, create drawing (2013), and used flat pattern view. The tangent lines were projected and converted to centerlines, no customization (although you could). I don't have access to a copy of SW2021 to test for comparison, thanks SolidWorks. not
-Christian
2013!!! My favorite version!!
You created an example of using "Sketched Bend" for MB107. Your example and the description I gave using construction lines should work for MB107's needs. As you get to sketch a line, you get to dimension the line.
For anyone that's been a GI, SolidWorks has a program to purchase an SEK kit: https://www.solidworks.com/media/mil...cation-program
Also, Dell has refurbished workstations from time to time that usually are up to $800 to $1000 cheaper than new. I picked one up last year that had it been new, it would've been almost $2100 before taxes. I got it for $1241 before taxes. It even came with 3 years of a warranty service: https://outlet.us.dell.com/ARBOnline...s=dfb&frid=189
I hope I didn't break any forum rules!! :)
Words of wisdom, and I'd go even further and state that it is not "good engineering practice" to dimension bend lines or even the flat patterns themselves. The engineering drawing is a legal document that specifies your engineering intent, and as such should reflect the dimensions of the final part. IMHO the flat pattern has only two simple functions: 1. Confirmation that the part can in fact be manufactured using sheet metal, and 2. To present a suggested flat pattern that helps the manufacturer to estimate how much raw material to prepare, and the flat pattern should be marked as such on the drawing.Quote:
Originally Posted by FloydHankers28
And last but not least, a dimension to a bend line is impossible to measure in the final part, so the manufacturer can't produce a COC (Certificate Of Compliance) and you yourself can't measure it either.
Jeffrey-
I understand what you are saying. But, for the homebuilder, since we are not industrial designers for our home projects, I find it useful to be able to scribe a line at the theoretical bend midpoint to put it in the brake. Not really worried about the 'legal' engineering intent; I just want to take my CAD out to the shop and make a part. I even commit mortal sins like putting the same dimensions in two views, so I don't get confused, which happens easily. And sometimes I will put in reference dimensions over the dimensions of intent, just so I don't have to do the math out in the shop. So if I were being judged by good engineering practice codes and industrial compliance, I would fail miserably, but I am having fun and building stuff, with my somewhat imprecise machine tools, but the final result is a usable part. That's why I pay myself the big bucks :-)
And just trying to help out other learning CAD guys, since at my shop, I AM the engineer, the CAD guy, the Machinist, and the fabricator, not to mention the test pilot and the pool boy.
-Christian
Hopefully you don't mean "scribe a line" literally. That is very poor practice. I do agree that flat patterns are valuable for us as homebuilders.
fine point Sharpie.
Did anybody find a solution?
I'm having the same problem in 2022.
Further to this, only parts created in 2022 have this issue. If I open (using 2022) a part created in 2021 I can select the bend lines. This seems to point towards a document properties setting.
For Christian and all others who want to get hung drawn and quartered, shot at dawn and then asked to leave the country, all because they disobeyed "good" engineering practice, I looked up the following in Help: "Drawings of Sheet Metal Parts". Also contrary to good engineering practice I followed the instructions and produced the following part and drawing: