Creating flat patterns from solid models

[Anonymous]

Hey guys,

Really struggling here and its doing my head in. Ive seen it done. Ive watched videos and it just isnt making any sense to me and im pulling my hair out at work here.

I am converting an autocad 2d file I have into 3d. Originally I would calculate the flat patterns and just draw and end view with dimensions to send off for pressing. Now I want to get the file converted to 3d and have inventor do flat patterns. 

I have copied and pasted the end view into inventor, extruded it as need be. I now have a solid shape of the item. How do I get this to turn to a flat pattern? I know its something simple I just cant get it to work. Ive tried reading all that I can and watching videos on youtube but no one seems to do a shape like mine which is where I think im losing what to do. 

If anyone could help it would be very much appreciated as I have about 10 different pieces like this to do. Have attached the file. Also going from 2013 to 2017 probably isnt helping and I dont think work is likely to put me through a course to learn.

Thanks

Brad

[blair · Accepted solution]

To start, you don't have a uniform material thickness. The all the "corners" don't have a uniform thickness. IV2017 now allows for "sharp" corners but only one side of the corner can be sharp. You have sharp inside and outside corners, this means the material will be thicker at the corners than on the flats. If you create inside fillets and outside fillets that have a radius that's greater by the thickness of the material, then the items will flatten.

The other issue is with your thickness of the material in the part. One of the legs has a thickness of 3.943mm and two other legs have a thickness of 3.932mm while your Sheet-Metal Styles is set for 4.0mm.

If you fix these issues then your part will flatten.

[Anonymous]

Thanks heaps!! 

In autocad it shows as all being 4mm. I tried radiusing the corners but obviously the flat sections still werent all 4mm. Got it working. Now to try some more parts. 

Is there any easy way to copy everything across? Got a lot of learning to do. I havnt done much 3d work since I did my qualification in 09. Only actually been working as a draftsman for the last 6 months. Was a foreman before that and got thrown in the deep end at work and was basically sink or swim

[JDMather]

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@titanmfg wrote:

In autocad it shows as all being 4mm. 

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Attach your AutoCAD dwg file here.

I will wager that AutoCAD will tell me otherwise.

[WHolzwarth]

IMO, the easiest way is using Sheetmetal's Contour flange.

Only one face contour needs to be sketched, bends are placed from themselves. See 2017 file

Walter

[blair]

I would agree with "WH" on this one. Simple sheet metal items such as this are easier to create from scratch.

Start a new Sheet Metal part, create the first face/leg of your part, then place a sketch on the end face of the part, create a line from the inside end corner that will follow the inside face profile of your part. Use the Contour Flange tool to select the line first, then the edge the profile will join to and you will have your flattenable sheet metal part.