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Square to Round Transition Options?

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Message 1 of 28
jeanchile
5660 Views, 27 Replies

Square to Round Transition Options?

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.

1_4 in Transition.jpg

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?

Inventor Professional
27 REPLIES 27
Message 2 of 28
stevec781
in reply to: jeanchile

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)

Message 3 of 28
jeanchile
in reply to: stevec781


@stevec781 wrote:

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



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.sinlge plate model.jpg

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?

Inventor Professional
Message 4 of 28
stevec781
in reply to: jeanchile

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

Message 5 of 28
IgorMir
in reply to: jeanchile

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.

Web: www.meqc.com.au
Message 6 of 28
jeanchile
in reply to: IgorMir

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.

Inventor Professional
Message 7 of 28
stevec781
in reply to: jeanchile

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.

Message 8 of 28
jeanchile
in reply to: stevec781


@stevec781 wrote:

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

 


I know. I can't explain it.


@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.

 


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.

 


@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.


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.

Test 6 Worked.jpg

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

 

Thank youSmiley Very Happy!!

 

Inventor Professional
Message 9 of 28
IgorMir
in reply to: jeanchile

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!Smiley Happy

Regards,

Igor.

 


@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.

 

Web: www.meqc.com.au
Message 10 of 28
jeanchile
in reply to: IgorMir


@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!Smiley Happy

Regards,

Igor.

 

 

 


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 Smiley Frustrated... specifically the guy running the press, everybody else agrees with the way I would normally do it.

 

Thanks again for the help!

Inventor Professional
Message 11 of 28
mrattray
in reply to: jeanchile

My shop does it the same way. I actually wrote a couple of simple "programs" for generating transitions. Mine get the little corner cut out thing, but they don't show up on the blanks so I just ignore it.  The file that stevec781 posted has a funny looking blank, look at the corners, they're all splined up. I don't know if that actually matters to you, but my laser program wouldn't be able to process that.

I don't remember how I coded the drawing side of it, it might not work without my default.ivb file. Let me know if you want the code from that (if there is any).

I also made some for rect to rect and round to round if you're interested in those I'll post them.

 

Mike (not Matt) Rattray

Message 12 of 28
jeanchile
in reply to: mrattray

Thanks for posting the files. Unfortunately, I can't open the files because I am on 2011. That being said, I have a workflow that mimics the fabrication process. I do get the funky shaped corners though but that hasn't been a problem in the past. When I put the first attempt I made into an assembly I get corners that interfere with each other too and I'm not sure what causes this:

Corner Interference.png

 

At the end of the day, I think the workflow that Stevec781 gave me (not the file he posted) is the correct way to go about it. I just wish I could see how you are doing it. We always wait until the next version is announced before we upgrade to the previous one so I should be running 2012 soon. I'll have to come back and take a look once we upgrade. We only do these transitions once in a great while so on the next one I can come check back.

 

Thanks for the help!

Inventor Professional
Message 13 of 28
mrattray
in reply to: jeanchile

It looks like tt's the way you're mating the parts. Remember that they're still flat sheets butted together.

This is what mine looks like:

trans joint.jpg

Mike (not Matt) Rattray

Message 14 of 28
jeanchile
in reply to: mrattray


@mrattray wrote:

It looks like tt's the way you're mating the parts....



Yeah, that's what I thought at first too but it's not. The files I created were done so around the origin (like a skeletal modeling technique) and then circular patterned around the axis. All the dimensions of the transition are perfect but the corners are hitting. It's the reason I scrapped this method in the beginning. Thanks for the help though. I'm anxious to see your workflow one we upgrade.

 

EDIT: The file I am talking about is the TEST 1 file I put up in my OP in case you are curious.

Inventor Professional
Message 15 of 28
mrattray
in reply to: jeanchile

Reverse the direction of the lofted flange feature and you should be in the money.

Mike (not Matt) Rattray

Message 16 of 28
IgorMir
in reply to: jeanchile

Hi Jean,

Here is a brake press version. Since I am still  with IV2010 I had to use Delete Face feature. That produces a neater model but on the flat pattern you will see an excess of material in the corner. If the Delete Face feature is suppressed - the Flat Pattern is good as gold but the model is showing a notch in the corner.  Maybe the latest release of IV is handling that transition better, but for the IV2010 I would convert that part into iPart and suppress the feature in one child. Just for the Flat Pattern creation.

Regards,

Igor.

 


@jeanchile wrote:
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.

 

 

Web: www.meqc.com.au
Message 17 of 28
jeanchile
in reply to: mrattray


@mrattray wrote:

Reverse the direction of the lofted flange feature and you should be in the money.


I can't. It needs to be 2'-4" square and 10 3/4" round at the outside, not the inside. What did I screw up?

Inventor Professional
Message 18 of 28
jeanchile
in reply to: IgorMir

Igor,

 

On my computer your part doesn't completely flatten all the way and I can't figure out why. Does yours go completely flat?

Inventor Professional
Message 19 of 28
mrattray
in reply to: jeanchile

Then subtract two material thicknesses (actually use 10.75-Thickness*2 for the parameter so it stays parametric) from the dimensions and reverse the direction so you're modeled to the ID but you'll still get the correct size.

Mike (not Matt) Rattray

Message 20 of 28
jeanchile
in reply to: mrattray

As with most of my endeavors, it's not that easy. First, let me state that I am by no means attempting to "split hairs" or be a "pain in the you know what" because I already have a work flow that produces usable results that I am thankful for and I appreciate all of your input because I am eager to learn some of the ways others would do this.

 

That being said, I can't simply subtract the thickness because the thickness is the "hypotenuse" of a triangle that would require the "base" to calculate correctly. If I offset the 2'-4" dimension by the thickness my outside will be smaller than the 2'-4" (the difference between the "hypotenuse" and the "base" of the triangle). I can obviously figure it out using another sketch, or a calculator, or whatever, I was just trying to follow the JD Mather school of thought and not do more work than was necessary Smiley Wink.

 

If I get some more time here this afternoon I will try to work up an example of what you are talking about working to the inside (which is where we would normally work anyway, this piece mates to another vendor's equipment hence me working to the outside).

Inventor Professional

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