I have a blank length of round stock and I need to form it at 90 degree angles. What command can I use to do that?
One way to achieve this is to draw the L shape and Extrude it square and use Sheet metal commands, then for visuals add a fillets to make the final shape round
You have to suppress the fillet when you flatten
Why not use a Sweep to create it in the desired shape to start with?
That's an extra sketch
Thin extrude = 1 sketch
Sweep = 2 sketches
Either way works, right
Adding Sheet metal is extra features, but with the deal you get a flat pattern and a bend line.
To create a bend in a cylindrical shape, you could try one of the following -
Model the bend using the swept boss feature: 2015 SOLIDWORKS Help - Creating a Sweep
You could bend an existing model using the flex feature: 2015 SOLIDWORKS Help - Flex Overview
Or there are a couple of other ways if neither of these give you what you want.
Flex is just what I was looking to do. I have a 3/4" round stock, cut to 29.325" length. The radius changed from 1.75" to 1". I am making a handle and I have to put two equal bends at 90 degrees and maintain an 18.05" on centers dim.First time working with flex.
I have one flex in the part, but am having a hard time controlling a second flex. HELP!?
Can you please show some pics of the issue you are having? Also, if you already know your specific requirements, Glenn's advice would be strongly suggested.
Everyone either has a new feature they like to work with or something that they are comfortable with, I'm a sheet metal guy so I'm gonna pick sheet metal features, very robust, multiple bendings no issues, plus you get bend lines...
Understand the desire to have a bend line on this......however, I would put a flex command at the very bottom of the list for a geometry construction tool.
The beauty of using SolidWorks - is the options that you have to create any design, however there are definitely a lot of tools you can use and yes the Flex Tool is one of them.
I have probably gone backwards a few times and kind of stayed in that rut when it comes to using certain features, because of getting burned with half baked features when they were released. I had a really bad experience with edge flanges and certain sheet metal tools that came out in the past, however today all is fixed, but I still tend to extrude model the pc and then add my bends and the same with other features.
Having said that - I still would grab for SW long before AutoCAD and Inventor.
Flex can be a little finicky, especially with more than one in a part. For more control you might see if the Deform feature, using curve to curve will work for you. LIke Flex, it has lots of options and settings and you often just have to try several times to get just what you need.
Erik,,, that is so cool. I had no idea you could use "Deform" like that. Thank you for showing me. I noticed you did have a typo 19.05 instead of 18.05. I also notice the the inside radius is .002 off. Not sure what would cause that. I also noticed that the length of the "Boss-Extrude" (29.325) has nothing to do with the total length of the part but Sketch2 does. Since this was under defined (vertical legs) I stretched them out and the deform followed. I didn't expect that.
You can bet I will be using the deform tool more often now. Got to study this some more.
I was just trying to toss out an example. I have to admit not checking it over at all before I posted. As i've mentioned before, Deform is one of those "often overlooked" features, it seems to get lost behind the splendor of Flex.
I like what John did. Since you are starting out with a fixed length of 29.325" and have a hard dimension of 18.05 you will need to know what the legs are going to end up at. If you do a flex on this it will be wildly unrealistic (no stretching, no compressing). I used a sheet metal "Swept Flange". Of course it has to be tubular but I figure once you get the leg dimensions you can do a solid sweep (non sheet metal) if you so desire.
After more thought I would suggest forget about any sheet metal, flexes, or deforms. Just do as Glenn suggested and with two sketches do a solid sweep. You know what the overall of the round is, so for the path sketch give it a path dimension equal to your overall and make the legs equal. That is what I did in my first pic. That makes the neutral axis at .5 the material thickness which is reasonable. If you really need to dial in the leg lengths I would suggest bending a part and determine the bend deduction. Then from that determine the neutral axis from a bend calculator. I'm sure who ever is bending this can let you know what the neutral axis should be. Then do a path dimension on the neutral axis and let that drive the swept path.
I would expect you don't need to do anything other than define the profile and path. You have two "fixed in stone" tangent edges (between the bends) and any bender can use that. The legs length will end up wherever it ends up. Keep in mind they will be shorter than when you used a 1.75" radius since you are sucking up more material. I also suspect they will be cut to size after bending (maybe wrong).
Now I'm going to look into Erik's part. I'm bound to learn something.
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