Hole in flat pattern of cone

[hawkerxj]

I have a cone shaped part and would like to put a hole in the curved face. I would like have to hole square to the face in the flat pattern so it can be cut on the plasma table, is there a way to do this? I attached the part with holes in the approximate location.
Thanks
Mike Hawker

[JDMather]

Several solutions depending on exactly what you want. This is my first guess.

Wait a minute, did you state what release of the software you are using?

[Anonymous]

Mike,

You want two circular loops or the current intersection loops?

Jacob

[hawkerxj]

Using IV 11 Pro, sp3

[hawkerxj]

I'm looking for something that would produce a flat pattern like in the picture attached. The two circles were sketched on in the drawing in this case
Thanks for you help,
Mike

[JDMather]

I don't have r11 but you do realize that if the holes are circular in the flat pattern they will not be circular in the folded model. The desired finished shape and the perpendicular cut are two different problems.

[hawkerxj]

I realize that, the holes are only for lifting the cone and don't have to be perfect circles in the folded model. The perpendicular cut holes cause problems with our old plasma table. I placed the perpendicular cut holes to show the desired location.
Thanks for your help Message was edited by: hawkerxj

[JDMather]

Use Split with the circle sketch to split the face. Then Thicken with Cut option to cut the holes. You can change the shape of the sketch if needed.

[hawkerxj]

Thank you, that worked perfect.

Mike

[Anonymous]

Hi! Did you try cut across bend?

Johnson Shiue
Inventor QA Tech Lead, Autodesk
johnson.shiue@autodesk.com
wrote in message news:5792036@discussion.autodesk.com...
Using IV 11 Pro, sp3

[JDMather]

>Hi! Did you try cut across bend?

Would need a planar face on which to sketch.
Can you post an example solution for this part?

[Anonymous]

The solution I have is a hack. I will add a small flange (planar face) on
one side and create a sketch based on teh flat face. Project flat pattern.
Then add two circles to the sketch. Next, cut across bend using the two
circles. Lastly, use Move Face or an Extrusion to remove the small flange.

Johnson Shiue
Inventor QA Tech Lead, Autodesk
johnson.shiue@autodesk.com
wrote in message news:5792350@discussion.autodesk.com...
>Hi! Did you try cut across bend?

Would need a planar face on which to sketch.
Can you post an example solution for this part?

[RANDYWINDERS]

I know this is a really ole thread but I am having trouble with this. I created a cone using revolve and converted it to sheet metal. I can flatten the cone but i need to cut a hole in the cone for an access door. I projected the flat pattern and sketched my door but the cut across bend fails.

INV2009

I know the version is old but its what i've got to work with.

Any help would be greatly appreciated.

P.S. I first tried a surface loft and thicken but couldn't flatten it.

I have attached the ipt here.

[JDMather]

I would recommend against using Fixed Constraints.

Create a single angled line sketch (no rectangle).

Revolve as a surface.

Create Rectangle on one of the origin planes as appropriate.

Use the rectangle to trim the opening in your surface.

Thicken your surface.

[RANDYWINDERS]

JD, The reason for using fixed constraints is that i need to match the id of a cylinder at the top of the cone that is 3/8 thk and the od of a cylinder at the bottom that is 1/4" thk. What you didnt see is the rest of the cyclone. I'm working of your soilution. I'll let you know how it turns out.

Thanks

[JDMather]

I would use dimensions or projected geometry - not Fixed Constraints.

I still don't understand the reason for Fixed constraints.

Where did you get your construction lines in Sketch1?

Import from AutoCAD?

[RANDYWINDERS]

Actually the fixed points and construction lines were projected geometry from the assembly this part goes into so I guess I did it as suggested. Your process worked out fine. I had to adjust the dimensions of the door cutout a bit to get the desired 12x12 cutout because sketching the door cutout on an origin plane caused it to be off because the sketch isn't parallel to the surface to be cut. But a little fiddling and it works just fine.

Thank you for your help.

[JDMather]

You could create a plane tangent to the conic surface for the sketch.

[RANDYWINDERS]

Yea that would get me closer but still need a little adjustment. What I really need is to convince the boss that we need to upgrade to 2014