Creating a flat pattern from a loft

[Anonymous]

Hello,

I can't make a flat pattern from a loft.

First of all, I did get a model (11951-222505_022.ipt), but I don't know it's extension, but Inventor is opening it (and i did save it in .ipt), then I wanted to make a flat pattern from that weird model, but it didn't work, so I did tried to make myself one, simillar (Part4)

First I made a sketch, then another sketch, lofted it and that's it. What am I doing wrong?

[kennyj]

Hello!

Without opening your files I am going to assume several things:

1) that you didn't shell or make the part hollow / have thickness?

2) that you didn't set your sheet metal thickness default to match the actual model thickness exactly?

3) that you did not Rip a seam for Inventor to know where to start/stop the fold  (If you fold this out of paper, where do the paper's outside edges meet? Did you show this on your model?)

Take a look at this video and see if it helps:

https://www.youtube.com/watch?v=p5Qm-MQBQng

Hope that helps,

Kenny

[salariua]

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@Anonymous wrote:

Hello!

Without opening your files I am going to assume several things:

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@Anonymous you have a couple of issues to fix before following @kennyj 's advice.

original model (11951-222505_022.ipt) has a thickness of "27.806619754 mm"

new model (Part4.ipt) has a thickness of "36.587634256 mm" and rule set to "40mm"

[salariua]

@Anonymous it does work ... Take a look at my attachment and repair the end cut. I don't' have time to properly fix it but this will get you in going in the right direction.

[JDMather]

@salariua

iProperties indicate Inventor 2013.

[JDMather]

@Anonymous

You can simplify your sketches as single arcs.

Then use the sheet metal Lofted Flange tool rather than standard Loft tool.

Be sure to set the Output to Die Formed.

[salariua]

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JDMather wrote:

iProperties indicate Inventor 2013.

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my bad... should have checked, thanks for that @JDMather

[Anonymous]

Hello,

The problem is that these are not both arcs, one is an arc (element no. 2 - see picture 1) and one is a kicked elipse (element no. 1 - see picture 1)

These are steps I did:

1. Open a model.

2. Made a drawing, after that a section - to see these funny elipse (element no. 1 - see attached pic 1).

3. Make a sketch on .idw, project this elipse on sketch to copy it and  finally copy it.

4. I did open a new part, make a sketch and paste this copied elipse.

5. Inventor consider it as a spline.

6. I made a second sketch, on the offsetted plane - circle shape (element no. 2 - see attached pic 1)

7. Lofted flange does not see the profiles.

Part 1: My new sketches.
Model: Basic model from which I want to copy the shape of this elipse.
All I want is to make a flat pattern of a element no. 3 - see picture 2, including a triangles.

[Anonymous]

A misssing PICTURE 2 

[Anonymous]

@JDMather, @salariua

[salariua]

Let's try this again. Are you trying to get flat pattern of this part?

EDIT:

is this what you're after:

[Anonymous]

Yes, I want to try make a flat pattern of that part. But I can't for instance convert it to sheet metal.

There is an error: "This model cannot be converted to Sheet Metal because it contains features that have created multiple bodies. In order to convert to Sheet Metal these features must first be removed".

I wanted to isolate this part, but my Inventor can see it only with connection to pipe. 

I can see a Thicken1 option in your browser, you first apply a thickness and then in sheet metal defaults you set this thickness to make a proper flat pattern?

@salariua

[S_May]

Hi @Anonymous,

[salariua · Accepted solution]

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@Anonymous wrote:

Yes, I want to try make a flat pattern of that part. But I can't for instance convert it to sheet metal.

I can see a Thicken1 option in your browser, you first apply a thickness and then in sheet metal defaults you set this thickness to make a proper flat pattern?

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@Anonymous I have indeed used copy on the inside surface and then thicken the quilt to a measured thickness of your model.

I don't have access to 2013 here and I won't for a couple of hours but I will do a screencast in 2015 and hope it's close enough for you to follow in 2013

Ideally, you would want to derive the model into separate parts and not use copy as I did just so that all the parts update when the original model changes but it might not be the case here, seems to be a one off.

See this video here

[Anonymous]

It works, thank you very very much!:)

Have a good day!

Best regards

MRumin

@salariua

[Fletcher_Apel]

Hi @MRumin

Thanks for the video it was great, I tried a few methods including exactly as you showed however I am still stuck. I want to produce fabrication plans for a lofted chute going form a 1400 x 400 mm rectangle to a 250mm dia circle, with a 10mm wall. I have tried to complete this as 1 part, 2 parts, and for part and it never flattens out. 

Thanks

Fletcher

[JDMather]

@Fletcher_Apel 

You have replied to an ancient thread.

Attach the *.ipt file of your attempt and indicate what version of Inventor you are using.

Did you include a rip in your profiles?

[Fletcher_Apel]

I'm on 2021, I have attached the files

[kennyj]

Please start your own post with proper title and tags so others can help you (and get the same help if they have the same question after you figure it out).  Thank you.

[JDMather]

See Attached possible solutions.

In the file that you attached - you did not use Sheet Metal tools.

Your Sketch2 was unconstrained?