helix cut out of sheet metal cylinder (not thread)

[Anonymous]

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

[JDMather]

You didn't include any dimensions in your figure or attach any trial attempt ipt files?

Is something like this what you are after?

[Anonymous]

Sorry I didn't think of giving dimentions as it the method I want to try and learn rather than actuall just get this one done... There wasn't any reasonable trila ones except for the flat plan above . I had loads of failed attempts but to be frank they would have confused the issue had I have posted them 🙂

Anyway without any further info you have got it in one . that is the exact thing I am trying to do....

Could you give me a few tips on how you did it please.

Thanks

[Anonymous]

I had marked this as solution found but was worried it would then prevent any further posting on this thread. I will of course re do the solution found thing as it is the exact solution. I've just got to find out how you did it now...

[JDMather]

I will not be at 2013 machine till tomorrow.

There are several ways.

Wrap to a surface, trim and thicken is one technique.

[Anonymous]

Thanks for helping out I have had a quick look at the areas you mentioned but it is still not clear to me. Sorry 

If you do manage to get near a 2013 machine (or older I guess) and manage to do a quick few point lesson I will be very happy indeed.

I intend to take this to a laser cutter near me so I do need to work from flat patterens or solids and turn them in to flat patterns...

Thanks

[JDMather]

You will have to determin the k-factor for your material.

see attached example

(I should have written Split rather than Trim in my previous response.)

[Anonymous]

Hello, yep that example looks great.

I was hoping to use the standard material of galvanised steel as that's what I'll be making the part out of, that sets things like K value doesn't it ?

I may be being a bit slow here but is there any way I can see how that example was made from the ipt ? I can see to component that have gone in to it and of course I can change the sketches and make whatever size bit I want, but I would really like to know how to do it....

Thanks....

[JDMather · Accepted solution]

Right click on the Flat Pattern and delete it.

Drag the red End of Folded marker to just below Sketch1 in the browser.

Start  a new part file and recreate Sketch1 from scratch.

Post back for the next step when this is done.

[Anonymous]

do you mean just a line 25mm tall ? or include the other things in it like a revolution .

[Anonymous]

What I mean by the above is that when I move the stop mark up (handy thing I didn't know) it hasn't only got the sketch 1 showing in the menu it also has a surface body folder but everything in it is greyed out so I'm guessing ignore that at this point...

[JDMather]

---

@Anonymous wrote:
do you mean just a line 25mm tall ? or include the other things in it like a revolution .

---

Sketch1 and only Sketch1 (4 lines, 2 dimensions).  (the 4 lines created with the Rectangle command)

[Anonymous]

ok done that.

[JDMather]

Drag the red EOF marker down one step to below Work Plane1.

In your new file create a workplane perpendicular to the XY plane by selecting the XY plane and the vertical object line from Sketch1.

[JDMather]

In my example drag the red EOF marker to below Sketch2.

In your new file

Start a new sketch on this new plane and Project Geometry the vertical object line from Sketch1 then change it to construction.

Add the other three lines and dimension.

For the horizontal line enter the dimension by clicking on the Diametral dimension in Sketch1 and *PI.

This makes the baseline of Sketch2 equal to the circumference of the circle.

[Anonymous]

ok

[JDMather]

In your part drag the red EOF back above Sketch2 and Workplane1 so that only Sketch1 is visible.

Revolve a Surface Body 359.99°.

[Anonymous]

Opps I haven't got a diametric dimension I've only got the height and length of the rectangle ie 25mm and 50 mm. where does the 100 diameter come from ?

[JDMather]

In your file

drag the red EOF to below Sketch2.

Start a new 3D sketch and select Project to Surface.

Select the surface as the Face and the angled line from Sketch2 as the Curve.

Set the Output to Wrap to surface.

[JDMather]

When you select a sketch centerline type (not the endpoint of the centerline) and then anywhere on the construction line you will get a diametral dimension.

Do you know how to change the linetypes to construction and centerline?

If at any time your sketch does not look EXACTLY like mine saying OK is not the correct response.

Post file and ask questions.