Sheet metal lofted flange problem

[benhVQ499]

Hi,

Apologies in advance for the noob question - am pretty new to Inventor...!

I'm trying to draw and develop a sheet metal mould part in two pieces, an inner (Part 1a) and outer (Part 1b) that will be welded together to form the finished part. The outer part lofts correctly but when the inner fails when I try the same thing - what am I doing wrong???

   

[johnsonshiue]

Hi! Please zip up the part and share it here. The forum experts can help take a look.

Many thanks!

[S_May]

[benhVQ499]

Hi,

Sorry - thought I attached them to the original post. Please see attached.

[benhVQ499]

Hi S_May,

Thanks very much for your help but my part is slightly different - the cylindrical shape tapers conically top to bottom, and the angular gap is not quite perpendicular to the circular face (ie. the flange face lines do not converge on the arc center).

Have attached zip of my models so far, would really appreciate any guidance....

[IgorMir]

Hi Johnson;

Interestingly enough - Inventor seems to having a problem with that particular design. Here is a quick representation of the OP file. So far - I am struggling to get the shape I want. As can be seen in the file - the Lofted Flange is producing something different to what is expected. Yet a simple Loft is quite happy with the geometry. Except, that at the end of the day I can not get a flat pattern from it, using sheet metal tools.

What's your take on this one?

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@johnsonshiue wrote:

Hi! Please zip up the part and share it here. The forum experts can help take a look.

Many thanks!

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[IgorMir]

Hi Ben;

Here is somewhat working model, but more review is needed non the less. Files are in IV2020 format.

Cheers,

Igor.

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@benhVQ499 wrote:

Hi,

Apologies in advance for the noob question - am pretty new to Inventor...!

I'm trying to draw and develop a sheet metal mould part in two pieces, an inner (Part 1a) and outer (Part 1b) that will be welded together to form the finished part. The outer part lofts correctly but when the inner fails when I try the same thing - what am I doing wrong???

   

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[benhVQ499]

Hi Igor,

Thanks for your help. Your approach is one I hadn't considered and looks promising, will continue with it to try and get a full solution..... 🙂

Any idea why it might be failing initially? Is particularly frustrating as the outer component lofts and develops wthout any problems.

Cheers,

Ben

[IgorMir]

Hi Ben;

Here is a fresh set of files. I have started from scratch just to eliminate the possibility of file's specific errors. Yet, as can be seen - the outcome is pretty much the same as in the previously sent files.

The outer shell is happy with the Lofted Flange - with the output as a Die Formed or a Press Brake one. The inner one, however - can only accept the Press Brake output.

Another thing I have noticed is that the side flanges for the Outer shell can although follow offset on the Sketch2. But not the  side flanges on the inner shell. In there top and bottom sketch lines for the flanges got to be aligned with each other for the Loft Flange to work.

At this point of time I am hesitant to offer any explanation for the phenomena. Let's wait and see what other members of the forum can come up with.

Cheers,

Igor.

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@benhVQ499 wrote:

Hi Igor,

Thanks for your help. Your approach is one I hadn't considered and looks promising, will continue with it to try and get a full solution..... 🙂

Any idea why it might be failing initially? Is particularly frustrating as the outer component lofts and develops wthout any problems.

Cheers,

Ben

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[johnsonshiue]

Hi Guys,

These are very good examples. I don't think Sheet Metal Lofted Flange is good at handling sections with change in convexity (concave to convex or vice versa). For this case, the only workaround I can think of is to use Loft Surface instead (remove the fillets) -> Thicken. Then the resultant part may not be unfoldable. You will need to use Unwrap to approximate it.

Unfortunately, there isn't a straight forward workflow to do that at the moment.

Many thanks!

[S_May]

[IgorMir]

Hi Johnson;

Thanks for looking into it, much appreciated.

It seems that in this quest we have unveiled some Inventor's limitation. To top up your collection of files, exhibiting the discussed issue, please find a set of four (IV2020 format) individual files. They all have exactly the same parameters. One of them, however, has the side flanges turned inward. While the remaining three have the side flanges pointed outward. The outcome can be clearly see in all the cases. I hope - the software developers might want to have a look at it.

Cheers,

Igor.

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@johnsonshiue wrote:

Hi Guys,

These are very good examples. I don't think Sheet Metal Lofted Flange is good at handling sections with change in convexity (concave to convex or vice versa). For this case, the only workaround I can think of is to use Loft Surface instead (remove the fillets) -> Thicken. Then the resultant part may not be unfoldable. You will need to use Unwrap to approximate it.

Unfortunately, there isn't a straight forward workflow to do that at the moment.

Many thanks!

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[S_May]

[IgorMir]

Thanks, Sacha;

Your model just confirms what I have found too.

Cheers,

Igor.

[johnsonshiue]

Hi Guys,

Many thanks for sharing the issues! There is definitely room for improvement, particularly in Lofted Flange. I will work with the project team to understand the behaviors better and see what we can do. Based on my limited understanding of how it works, I don't anticipate a quick fix.

Thanks again!

[JamesSlaven8282]

I experienced this issue in 2016 with a similar cone shaped design. It was incredibly frustrating as I thought I was doing something wrong. I finally did get lofted flange to work sufficiently for a reasonable flat pattern. The behavior has remained consistent ever since.

Today I pulled a copy of that old part to retrace my steps for a new design but while editing I lost the lofted flange and then ultimately fatally crashed Inventor. Luckily it was a copy but to date I have spent too much time trying to get the lofted flange to work on a leg-out flanged cone.

I believe my workaround involved the top and bottom arc centers not being on the same origin axis. I also sketched the flanges similarly to the examples earlier in this thread rather then adding flanges later with the flange tool.

Note:

1. Sketching the flanges will result in the Lofted Flange error message

2. Using Lofted Flange on just the top and bottom arc sketches (without flanges) does work but afterwards the flange tool will not create the flanges.

I have never posted on this forum so I hope to receive a ping if someone has a solution and replies.

[JDMather]

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@JamesSlaven8282 wrote:

I have never posted on this forum so I hope to receive a ping if someone has a solution and replies.

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@JamesSlaven8282 

Attach file here Reply to Message - Autodesk Community

[gmwi]

Make sure that your intersection of flange and arc are filleted to a minimum of the material thickness. It does not like 0.0" radius bends.

[JamesSlaven8282]

I spent some time with this again and my results are consistent so I am glad to share the part with some experts.

This file shows five sketched variations of a sheet metal, center-axis quarter cone with flanges. Each sketch pair has a different flange approach... three leg-out and two leg in, with and without sketch fillets.

• Leg-in version with sketch fillets
  • Required the fillet radius to be greater then the Thickness and even greater yet for an Inside Offset.
  • Press Brake and Die Formed output method works (providing above condition is met)

• Leg-in without sketch fillets
  • Press Brake and Die Formed both worked unconditionally

• Leg-out version with fillets
  • Neither Die Formed nor Press Brake output methods worked.

• The leg-out versions without fillets:
  • Press Brake method works
  • Die Formed does not work

Have a look. 

[JamesSlaven8282]

Thanks for the tip @gmwi
I increased the fillet radius bit-by-bit until I had no room for more but still achieved no success.