cant create flat pattern

[mgarcesUX9HW]

Hi im new to inventor I know theres still a lot to learn pls help i cant unfold the attached file, please help what im missign thanks! this 3d model was created in autocad 2020 and exported to inventor 2020. 

[Anonymous]

You're most likely going to want to recreate this in Inventor using the sheetmetal tools. This part does not have a uniform thickness so it will not be able to be flattened. I would recommend drawing the cross-section and using Contour Flange to create this part in Inventor

[JDMather]

Outside Radius = Inside Radius +Thickness

or

Inside Radius = Outside Radius - Thickness

[mgarcesUX9HW]

hi it supposed to be inside + thickness, maybe this was causing the error?

[mgarcesUX9HW]

but what would be the minimum bend raduis of a 0.5" thick mild steel?

[mgarcesUX9HW]

for this matter any autocad model will not work with inventor for flat pattern, i have a pipe also that wont rip same modelled in autocad

[SBix26]

An AutoCAD model should be able to be flattened in Inventor, but only if it is modeled correctly (absolutely uniform thickness throughout the model) and if the Inventor sheet metal defaults are set to the same thickness.  Also, of course, that all bends are conical or cylindrical-- formed by press brake or roll.

Please attach an example or two of AutoCAD models that you want to flatten.  Someone can demonstrate for you, if you tell us what version of Inventor you're using.

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Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn

[johnsonshiue]

Hi! To create Flat Pattern in Inventor, the body thickness needs to be uniformed. In this part, the thickness is not consistent in the bend zone. The quick workaround is to use Thicken/Intersect to create the uniform thickness. Here is what you need to do.

1) Go to 3D Model tab.

2) Click on Thicken command -> uncheck Auto-Blending and check Auto Face Chain -> select the outside face and set the distance to Thickness -> set the operation to Intersect.

Or, it needs to work from inside out.

The resultant body should have uniform thickness.

Many thanks!

[mgarcesUX9HW]

Hi I have tried this but it gives me an error

[mgarcesUX9HW]

Hi thanks! attached are the modelled in autocad

1. socketpl2.dwg = cant seem to flattened it

2. column frame = i need to create a cut template for the pipe but it wont even rip

thank you please advise

[mgarcesUX9HW]

im using

autocad version 2020

inventor 2020

[SBix26]

Here's your answer (forums won't allow me to paste or embed images today 😠). 

Inventor doesn't do "close enough" math.  It needs to be exact to a lot of decimal places.  I moved the two offending faces to exactly 1/2" using Direct Edit, and the channel flattens just fine.

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Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn

[JDMather]

The original AutoCAD geometry was not modeled correctly.

This image is of the edges of two "concentric" fillets in AutoCAD.

Those two horizontal lines should be overtop of each other.

I am zoomed wayyyyyyyy in...

[mgarcesUX9HW]

1. did you recreate it in inventor using 2s sketch or just modify from the model itself?

2. so i have to be .00000 accurate on my model? to be able flatten it 

[JDMather]

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2. column frame = i need to create a cut template for the pipe but it wont even rip

please advise

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Some of this geometry does not pass Inventor quality check.

Based on what we have seen so far - I would not trust any work from this AutoCAD user.

I would use the dwg only as reference in creating high quality geometry in Inventor from scratch.

(There is no reason that it couldn't be created in AutoCAD - but it is more difficult to figure out what the AutoCAD user is doing wrong and even to recognize their errors.)

On the other hand - with a complete parametric history - it is easy to diagnose issues and then avoid them going forward.

[JDMather]

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@mgarcesUX9HW wrote:

2. so i have to be .00000 accurate on my model? to be able flatten it 

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There is no reason you can't have .000000000000000 accuracy in AutoCAD.

[mgarcesUX9HW]

how can i check the parametric history from autocad model, i think this model was created from basic autocad extrude and solid to solid  subtract command

[SBix26]

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@mgarcesUX9HW wrote:

1. did you recreate it in inventor using 2s sketch or just modify from the model itself?

I did not recreate the channel in Inventor, I just moved the two inside faces and their adjacent fillets .00038 inches toward the outside using the Direct Edit tool.

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Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn

[JDMather]

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@mgarcesUX9HW wrote:

how can i check the parametric history from autocad model...

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Did the AutoCAD user use Parameters?

Did the AutoCAD user set DELOBJ = 0 ?

[mgarcesUX9HW]

unfortunately delobj was set to 3