How do I bend this tab? The sketch bend feature extend the line to the edges of the plate and bends the whole thing. I only want to bend the triangular tab.
I've never tried this but what comes to mind is cut out the triangle then use an edge flange. Also maybe if you move the sketch up so it is not right at the bottom of the triangle the sketch bend will not bend all the way across.
(I'm not at my computervright now so I cannot try these myself)
First method I described worked for me.
Even though I believe there is an easier way to do this here is one more method.
1) Create a triangle tab
2) Use a sketch bend to bend it up
3) Create a cutout tab around it.
Since this would be punched in reality, I'd suggest doing this using a form tool.
Im not in front of SW at the moment, but this is the first avenue I'd explore.
I still have a can opener that makes this kind of shape. But I like the idea of a form tool. I have not use that feature in many years.
I think something wrong with Sketched Bend feature because it works fine up to some condition.
I used split feature as workaround.
What caused the problem is the relief cut width.
Start to increase it until finding the minimum value.
The reason is that the excess material create self-intersection
When increased the width it works just fine.
Not in my case, I havn`t any self intersections in my model. SWX18 file is attached.
Unfortunately, I am using SW2016.
The other limitation is where the bend sketch pleased.
Move the sketch close to the triangle tip or reduce the bend radius and you will see the dependencies.
One more time - it is not my case
Please, build a model in this way.
What I am seeing from your screenshot is that the sketch is not on the right position.
Play with the attached file and you will see what I mean.
Sorry, I can`t agree with you. I don`t want to play with artificial offsetting dimension for bend line and I don`t want to have double edges in the corner, I need reliable way.
If you bend at 90Deg change the sketch dimension to be your bend radius + 0.1.
This will not affect the bend in real life.
Also, this is not an artificial offsetting but shows the real position of the bend.
In reality, if you bend it on position from your file it will pull up and stretch the corners.
This is a plastic deformation SolidWorks can't handle.
Hope this help.
Ok, it is not artificial, but 0.1 is artificial and if you decide to create mesh for FE calculation you will have problem with such tiny geometry
Yes, you are correct, it will affect the FEA.
That's why the step before FE Calc is to prepare the geometry for it.
I think it is good to have two configurations, one for FEA and one for drawing because the requirements of both are different.
OK, it was not so easy but I tried,
basically all my parts have two configs: solid and shell or solid and wire, hence, assemblies can have solid,shell and wire configs for example.
But configs don`t give you workaround.
This looks like a good use of the louver command. You can create the sketch and save as a block to use for future parts. Very useful tool for sheetmetal work.
Retrieving data ...