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Sheet Metal hole locations on a tube

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

We have a customer that creates a tubular sheetmetal part that is drilled with some holes.

Ordered mode.

The tube has a small cut in it so it can be flattened.

We need the locations of the holes in the flat but when we create a drawing we get splines or multiple arcs so we can't get to the center of the holes.

There is a setting on the Flat Pattern Treatment called "Maintain holes in flat pattern" but I still don't get round holes in my flat pattern.

Can any of you sheetmetal pro's confirm that this does not work? Is there a good solution?

Attaches is a part I was playing with. Not the customer part.

Thanks.

LMGi
www.TLMGi.com
8 REPLIES

Betreff: Sheet Metal hole locations on a tube

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Hi @JasonTitcomb

 

 

 

it seems as it has to do with the material thickness.

Reducing the thickness down (I tested it with 0.1 inch) will create circles again.

Maybe the thickness to diameter relation is to big for them.

 

But this is an issue I would involve GTAC and support

 

 

regards
Wolfgang

Re: Sheet Metal hole locations on a tube

Honored Contributor
Honored Contributor

Use small holes to find the center. After the part is flat, then recut the holes in the flat. (Unbend, cut, rebend)

Re: Sheet Metal hole locations on a tube

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

In a case like this, I would do it the same as @12GAGE describes.

Sean Cresswell
Design Manager Streetscape Ltd
Solid Edge ST10 [MP8] Classic [x3 seats]
Windows 10 - Quadro P2000
Testing: Solid Edge 2019

Re: Sheet Metal hole locations on a tube

Phenom
Phenom

Depending on the needs of the holes you'll need to use the suggestions already provided. I draw a lot of tube this way, as my laser cutter can only import a flat .dxf file. is your customer needing the hole locations to manually punch or drill? Remember you're essentially taking a bent part and expecting the hole to maintain shape when flattened, that wont happen.
I usually ask how is the part to be physically made before trying to give a answer on how to draw it.

Don't forget to set neutral factor to "1" when creating parts like this.

-Craig

Re: Sheet Metal hole locations on a tube

Honored Contributor
Honored Contributor

Attached is a screen shot of the design that raised the issue for me. The design is still very much in flux where the angled pipe is still moving around.

 

Setting K to 0 or 1 is not an options as the sheet metal parts have already been programmed in our punch/plaz and folder based on K=0.33. So the flat pattern can't change other than the location of the hole for the angled pipe.

 

What makes this even worse for me, is that our punch does not have a tool to create an ellipse. So if the part is thinner than 10 Gage (Punch vs Plaz), then I have to break up the ellipse into four arcs that are a great approximation of an ellipse. 

 

 

Re: Sheet Metal hole locations on a tube

Phenom
Phenom

@12GAGE wrote:

Attached is a screen shot of the design that raised the issue for me. The design is still very much in flux where the angled pipe is still moving around.

 

Setting K to 0 or 1 is not an options as the sheet metal parts have already been programmed in our punch/plaz and folder based on K=0.33. So the flat pattern can't change other than the location of the hole for the angled pipe.

 

What makes this even worse for me, is that our punch does not have a tool to create an ellipse. So if the part is thinner than 10 Gage (Punch vs Plaz), then I have to break up the ellipse into four arcs that are a great approximation of an ellipse. 

 

 

In your case there's no need to change  neutral factor, your tube/pipe goes thru a typical sheetmetal part (not a full radius rolled part).

In this case I'd create an intersection curve where the pipe crosses the sheetmetal and then create holes (punch shape) to best fit the area.

 

 


 

-Craig

Re: Sheet Metal hole locations on a tube

Honored Contributor
Honored Contributor

When you say an intersection curve, can you be more specific?

Are you talking about the surfacing tools? Is there a way to use the sufacing tools inside a sheet metal part?

 

I have never used any of the surface onyl tools. I'm 80% ordered sheet metal, and 10% frame tool and 10% typical parts.

Re: Sheet Metal hole locations on a tube

Phenom
Phenom

@12GAGE wrote:

When you say an intersection curve, can you be more specific?

Are you talking about the surfacing tools? Is there a way to use the sufacing tools inside a sheet metal part?

 

I have never used any of the surface onyl tools. I'm 80% ordered sheet metal, and 10% frame tool and 10% typical parts.


yes, under the surfacing tab, surfaces tools are available in sheetmetal. basically it'll create a curve at the intersection of two parts, for sheetmetal you'll need to select both faces of the plate and the o.d. of the tube. you'll need the intersecting part to be inter-part copied of course.

 

Below is a tube intersection an angle, curve is shown as it intersects all faces of angle.

junk.jpg

-Craig