helix cut out of sheet metal cylinder (not thread)

[Perfectg_uk]

Hello, My first time posting but I have been on here many times trying to learn a bit more from you fellows. I'm currently using inventor 2013 I generally mange to do what I need after a bit of searching and trial and error but this little problem has me stumped and I know it should be easy.

Anyway I have a flat sheet metal part

This is flat steel 1 mm thick. I want to bend it in to a cylinder so that the cylinder will end up with it's top cut in a helix. 

I can make a solid cylinder with wall thickness 1 mm then use the coil feature and this looks like it does the job and cuts right through the cylinder wall but I can't then discard the top bit. Similarly I can make a cylinder then rip it and unfold it in to a flat pattern but I can't then edit it.  Any suggestions on how I can achieve this would be most helpfully.

Thank you

[Perfectg_uk]

sorry , I'll have to go back to the start and try and figure this bit out it is asking me for an axis or it wants to revolve the 50 X 25 mm rectangle I've draw. To make matters worse I'm being harassed to get a job done. I bet you have much better things to do than to coach a numpty like me and I'll understand if you ditch me . But I'm gonna have to go for a bit.....sorrry again mate...

[JDMather]

Exit the 3D sketch.

Right click on Sketch2 and turn off Visibility.

Use the Split command with 3DSketch1 to split the surface body.

Thicken the surface body by the sheet metal Thickness.

You would be able to reverse engineer any Inventor file in this manner to see how it was created.

This is critical to learning Inventor (and is a really efficient way to learn).

[JDMather]

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@Perfectg_uk wrote:
.... it is asking me for an axis or it wants to revolve the 50 X 25 mm rectangle I've draw.

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..

My guess is that you did not change the other lines to Construction lines as in my example.

This is exaclty why I asked you to attach your attempt(s) here - your attempts would tell me what you do and do not know about using Inventor so that I know what to explain in detail.

[Perfectg_uk]

Thanks for being patient.

I have finally done it thanks to you.

One of my problems was the 100 mm diameter text on your Sketch 1. I'm still not sure where that comes from but I realised using 2 X the 50mm of my rectangle as the diametric for sketch 2 works just as well. The other thing I was getting in a muddle with was thickening before splitting because then it wasn't a surface it was a solid and I couldn't split and delete the bit i didn't want. Also if thickening first it would thicken the wrong way and make the circumference too big for the wrapped line to go all the way around. It seemed to work for me doing full rev rather than 359.59 degrees, it was by accident I forgot the 359.59 but it still worked so no probs. I guess as I made the first upright on sketch 2 (ie the projected line ) in to a construction line it didn't form part of the split tool so I had to add a line on the 3d sketch to close the gap.

Anyway once again thanks for your help and I hope my trials and tribulations will assist anyone else stumbling across this thread.

[JDMather]

Attach your final result here.  It sounds like you are still having trouble modeling the part correctly.

How does the Flat Patten look?

[Perfectg_uk]

Well I think it looks ok but here it is for scrutiny.

And the flat one

I've also attached the IPT...

[Perfectg_uk]

Hello JD does it look like I've done it right ?   What's the chances of me remembering how to do it next time   At least I'll have this thread to remind me.  Thanks for your help

[JDMather · Accepted solution]

It worked, but you did extra work because you revolved 360° requiring you to add a Rip feature.
And I would learn how to add diametral dimensions to sketches (pick the center line, not the endpoint of the center line).

[Perfectg_uk]

I'll have a read of the diametric thingys....and I now see the 359 degree rotation point... Thanks fellla

[JDMather]

When you do the Thicken feature set to the sheet metal variable Thickness.  That way, if you change the sheet metal thickness the part updates correctly.

And,  you didn't really need to Delete Face after the Split, you could simply Thicken the desired portion and then right click on the Revolved surface in the browser and turn off Visibility.

[Perfectg_uk]

Another couple of very handy hints..Thanks. I must admit I didn't know what the thickness thing in the sub menu meant, but that auto links to the thickness variable when you set the sheet metal defaults does it ?

[Perfectg_uk]

Sorry to be back again so quickly with yet another problem. I've made my two helix pieces and a truncated cone stuck on the bottom as per attached IAM. However I now want to put a cap on top of the sloping section ie between the two helix bits. I can extrude along the surface if I'm in an IPT but then I can't split it up again into separate parts. If I try and make a part in the IAM it wont let me extrude the along the face of one of the helix things. As per norm if anyone has any pointers then I will be most happy to hear them..... Thanks....

[JDMather]

Look at the size of the iam - 77k.

What is the size of your parts?

Do you think there is anything in your iam?

An assembly file (*.iam) is only a list of hyperlinks to the part files (*.ipt) and a record of assembly constraints (and a bit more).

You must include the part files.

[Perfectg_uk]

Ah I see, I haven't got a very speedy Internet connection and was pleasantly surprised it seemed to send it in a jiffy.... 

It wont let me attach all the parts in one go so I'll send the cone bit in the next post.

However the disc (PartC3d) and the cone (partEv2) don't really make much difference to my problem. It is just the two helix bits and putting a cap between them, closing off the sloping faces.. Thanks....

[Perfectg_uk]

and here's the cone

[JDMather · Accepted solution]

Is something like this what you are trying to create?

  If so, simply sketch a line of length between the inside and outside.

Create a Coil Feature and Thicken.

[Perfectg_uk]

That worked perfect , thanks.  I guess as its a strange shape I'm going to have great difficulties turning this in to a flat pattern ( In my minds eye it's not possible. SO maybe I'll snipe it in half and make two flat patterns. I think that should work unless there's a better way.

JD you are a very helpful and knowledgeable chap  I'm sorry to have taken up so much of your time. 

[Perfectg_uk]

Also as I'm cutting this out of flat and riveting it , has inventor got an automatic tab adder onner? I can add tabs by doing the rectangular or circular pattern and drawing one tab then multiplying it but I know inventor has some handy facilities like that built in...