Autodesk Inventor

[#1]

Hello all,

I have a square to round transition that I need formed up and the shop is telling me that they would prefer to split this thing at the corners rather than the flats. I've tried two different ways of doing this and I am looking for some input on how you guys would handle this part. It's 10.75" OD at the bottom and 2'-4" square at the top and 1'3" in length and made of 1/4" stainless steel plate. The shop wants this in four bent pieces that they can weld together down the corners.

I've tried making just the one side but I'm not getting the results I would like to see. Making the full transition (as in the picture above) gives the finished result I am looking for but I can't seperate it into multiple sides.

Any ideas on what else I can try?

[#2]

You could add a rip down one face of the full model and then add a cut feature to the flat pattern to leave just 1/4 of it.

(why they want to do 2 extra welds and try to get a bend right on an edge is beyond me)

[#3]

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stevec781 wrote:

...why they want to do 2 extra welds and try to get a bend right on an edge is beyond me

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Yeah, me too but they said it was easier that way. I split the last one in what I thought was the most logical place and they said doing it that way was too difficult and they prefer it this way.

That being said... I have to apologize for my ignorance with the sheet metal tools. It's not a function of IV I use often. I can't figure out how to accomplish what you are suggesting. I've tried the Unfold/Refold option but I can't select the bends of the lofted flange and I can't use the cut option in the flat pattern because it only works in the flat pattern.

I just need to be able to get them the one plate detail drawing but the assembly needs to show the quantity of four with the correct sizes in the BOM and I can't figure it out.

This is what I get when I model just the one side. The corners aren't right, they wouldn't be cut out like this in real life.

I've also tried trimming the solid (won't flatten) and ripping all four corners to get the flat pattern I need (but the folded model still shows all four sides).

I appreciate the help immensely. Any chance you can elaborate on your post above or help a guy out further?

[#4]

see attached, then just over ride the BOM qty in the drawing.

[#5]

I couldn't see Steve's model (his is a newer version of IV) but just in case here is what I can offer.

The full chute has to be represented as an assembly, of course. In the attached file I have left the Mirror feature below EOP marker, so you could have a look how the part will look like in the finished stage.

Best Regards,

Igor.

[#6]

Thank you both for the help with this issue. Both offer some ideas even though neither are the perfect solution for me but I can at least move forward with this task.

Stevec781, I see what you are talking about, thanks for the example. I actually have one attempt similar to this already but I was hoping for one where the quantity and mass was already correct without overrides.

Igor, your example solves the quantity and mass problems but it looks like the inside radius at two of the corners of the sqaure part are defined by you not by the sheet metal rules and I need to play with that a bit to see if I can get the result that would mimic the shop fabrication process of using a brake press.

They are doing this in quarters because the material hits the housing on the brake press if I do halves or the full thing. Normally I would do this down the flat face. This is one of those issues where my program wants to do this one way and the shop isn't going to do it that way. I understand why IV gives me the result I get when I just sketch the one side (notches at the corners) but it's not what will happen in the real world. What would be nice is if a sheet metal part would support multiple solid bodies and skeletal modeling.

I appreciate the help immensely. If you guys (or anyone else for that matter) has anything else to add I would be happy to hear it. You guys have been very generous with your time.

[#7 · Accepted solution]

Splitting it in the corners is 4 welds.  Splitting it on the each flat is also 4 welds. - no difference.

Splitting it in the corners will be a nightmare to press right on the edge of the plate.  Splititng it on the flats will be much easier to press to 90deg.  They shouldnt hit the machine on a 90deg bend.

You could try a very thin rip feature down the middle of the bend and then use an extruded cut to delete the unwanted pieces and then create your assembly.

Or you could create  your 1/4 model from middle of flat to middle of flat so that the full corner is in the part, then split it down the middle of the corner and then mirror the solid.

[#8]

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stevec781 wrote:

Splitting it in the corners is 4 welds.  Splitting it on the each flat is also 4 welds. - no difference.

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I know. I can't explain it.

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stevec781 wrote:

Splitting it in the corners will be a nightmare to press right on the edge of the plate.  Splititng it on the flats will be much easier to press to 90deg.  They shouldnt hit the machine on a 90deg bend.

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Yep. Seems logical to me as well. I spoke to the guy welding it up and he said it would be easier this way too because then he wouldn't have to brace it/tack it to the floor when he put it together. If the pieces were 90 degree corners they would stand up on their own and he could just weld the thing.

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stevec781 wrote:

Or you could create  your 1/4 model from middle of flat to middle of flat so that the full corner is in the part, then split it down the middle of the corner and then mirror the solid.

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This, however, worked like a CHAMP!! I wrote off the split tool when it didn't work in my second test but it worked on just the corner part. I would have never thought of this and I thank you for your persistance. Please go tell your boss that I said you deserve a raise.

I have attached the working part here for anyone who finds this in the future.

Thank you!!

[#9]

Hi Jean,

The corners' radius is defined by the sheet metal rules. It is equal to the Thickness of the material. Or double Thickness of the material if the Flange Loft goes inward.

To fabricate just a quarter of the chute would take pretty much the same effort in Inventor as to make half of it. But there is something bizarre is going on in your fabricating shop!

Regards,

Igor.

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jeanchile wrote:

Igor, your example solves the quantity and mass problems but it looks like the inside radius at two of the corners of the sqaure part are defined by you not by the sheet metal rules and I need to play with that a bit to see if I can get the result that would mimic the shop fabrication process of using a brake press.

[#10]

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IgorMir wrote:

Hi Jean,

The corners' radius is defined by the sheet metal rules. It is equal to the Thickness of the material. Or double Thickness of the material if the Flange Loft goes inward.

To fabricate just a quarter of the chute would take pretty much the same effort in Inventor as to make half of it. But there is something bizarre is going on in your fabricating shop!

Regards,

Igor.

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Yeah, I saw that. I was talking specifically about the brake press method where I have multiple bends at that corner. There isn't a perfect arc like in your example but a series of bends, bend lines, and inside radii that make up a spline shape. I appreciate the time and the help, I would have been stranded without the two of you.

And you're right... I haven't a clue as to what the fabrication shop is thinking ... specifically the guy running the press, everybody else agrees with the way I would normally do it.

Thanks again for the help!