Sheet Metal Bookend Creation Help?

mark_leger

Hi,

Trying to achieve a sheet metal model feature that can be boiled down to something like a bookend.
I've modeled a new bookend to experiment with, but I cannot get the middle tab to form properly.

            



I can't use a flange as it's 0 degree, and same for @MBartlett21 great Shaped Flange tool.
A sketch was created to then use the tab function, but while the Tab is not coming back with any errors, it's not formed either.

Here's a link to the document:
https://cad.onshape.com/documents/a0ed326b1a000dc74418e405/w/2c13dd39627b2b34ab3b461e/e/22cf18f3352a05182312ed4d

It could just be how I structured the creation of the part, but any help would be appreciated.

Thanks,
Mark

MBartlett21

@mark_leger
Would you be able to make the document public, so we can help you with it. At the moment, it is only shared via link.

matthew_stacy

@mark_leger,

I've been wrestling with these same kind of parts lately.  I started with a surface model, made boolean subtractions, and extended a surface boundary before converting to sheet metal.  This gets everything onto the flat-pattern, except for stiffening ribs.

I added those after finishing the sheet metal.  This isn't a particularly elegant solution, but basically works.

https://cad.onshape.com/documents/3a4e72796dec53b0c129cba5/w/7d90fdd10b35af7161694c3b

/e/8b25ddda98f39df0aa792956

 

mark_leger

@MBartlett21 The document in now public.
I made a new part to show how I tried to used your Shaped Flanges, but as you can see, it will only connect to one edge rather than two.

@matthew_stacy I will have a look at your document when I have some time today, but glad to see it can be accomplished.

Thanks!

bryan_lagrange

I would make and L shape sketch, sheet metal extrude. Then add a cutout through the tangent of the radius. Finally a tab at the bottom to make the book end shape.

mark_leger

@bryan_lagrange If you look at my model, your procedure is exactly what I did!  Only my tab is not forming correctly.
When you say "through the tangent of the radius," are you referring to the Right Face or Bottom Face tangent in your model?  Maybe my issue is just using the wrong face for the removal sketch.

@matthew_stacy I was able to make the part using your procedure, but you're right, not the most elegant solution.  



  

bryan_lagrange

@mark_leger here is the link to my model to show what I did.

https://cad.onshape.com/documents/d0a486096e15d852a3e103ee/w/8298067f2b805c945a866122/e/38af666d68f820549bf08c53

matthew_stacy

@bryan_lagrange very nice work. 

Would be great to:

• Notch the junction of tab and L
• Link dimensions of Sketch 3 to Sketch 2
  

matthew_stacy

I copied Bryan's model and started branch B1:  https://cad.onshape.com/documents/6aa160088e284fef5cdf3a09/w/28686668d7b0c38e3ecef512/e/280fd3af0f2f54730d922087

I added variables for the key sheet metal parameters so that tab length can be automatically calculated to match the cutout height (includes allowance for bend length).

Cutout height is also driven by variables. 

In my opinion this is a reasonably functional parametric model, but it requires a few cumbersome workarounds to make it all work.  I miss some of the tools in SolidWorks, such as the ability to reference every sketch dimension (e.g. "D1@Sketch1"), that would have made this a lot easier.

I would also like to have more robust sheet metal tools.  Onshape sheet metal seems to be rather finicky about tasks like mirroring and patterning features.  The "Notch" feature in this bookend model is an example.  I had to mirror the sketch entities.  I much prefer to mirror a feature rather than sketch entities.

mark_leger

Thanks @bryan_lagrange!
I had used the inside face rather than the outside face for the cutout and now the tab is forming correctly.

@matthew_stacy I specified Bend relief type in the sheet metal model and it created the notches for me, referenced those in the sketch for the tab.  Did not have to mirror anything.

I agree though that it would be nice to be able to reference sketches/set dimensions in the flat pattern instead of creating variables. 

Thanks again for your help guys.

steve_shubin

@mark_leger
@bryan_lagrange

Hi Mark — here’s another way of doing it

Of course Bryan’s model showed me how to use the TAB tool. So thanks Bryan

steve_shubin

@mark_leger
@bryan_lagrange

The above GIF has been edited

I eliminated a couple of steps (features) of the model

matthew_stacy

@Henk_de_Vlaam developed a clever approach to modeling this part that captures design intent with a very short, concise feature tree.  Check it out if you're interested:

• https://forum.onshape.com/discussion/14416/sheet-metal-tab-subtraction-scope-offset#latest
  

mark_leger

After playing around a bit more, I think @steve_shubin method is now the best way to make this part.
It's part 3 in my shared model, and stems from the conversation @matthew_stacy started in the link above.  You can sketch on the flat model!

It relates the cutout area to the tongue without variables and it accomplished in fewer steps.

steve_shubin

@mark_leger

Hi Mark — I’m happy to help with your model

If any one else is curious about this, below is the URL to the document

Also below are 2 GIF’s. The first which shows the different steps or features

The second GIF shows steps 4 and 5 in more detail

https://cad.onshape.com/documents/fd91f8e4eaa5abaf393e7ada/w/d12929a9d309270a39a63012/e/b92593ca4f504d2f5eecfb26