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punched/Drill holes on rolled sheet metal

Question asked by reeshi pradhan on Nov 30, 2011
Latest reply on Dec 1, 2011 by Erik Bilello

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Hi,

I am having a big problem.

I have hole on cylinder at equally distributed over surface. I have to wrap that cylinder with sheet metal as in attached file and also have to match the holes on rolled sheet metal to the holes on cylinder.

if I make holes on flat pattern at equal distance, it won't match to the holes on cylinder.

if I make holes on rolled sheet, it won't be practically possible.

So please suggest if there are better way to punch the hole on rolled/bent sheet.

Thanks in advance.

Reeshi

Denny Metcalf Dec 1, 2011 5:27 PM

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Hello Reeshi,

Don't worry, you are not bothering anyone. We help because we want to help, it's not a bother, lol. I'm just saying that if you want to get a very good answer, it's better to give as much description as possible so that we know what the problem is.

Here's a very fast and easy way to dimension without using reference geometry:

Place your flat pattern view and then draw a sketch on top of it making a bunch of lines that connect all of the holes together:

Then just dimension to the end points of each line segment.

When you're done, just hide the lines.

I use lines to emphasize that this method is a fast way, but not the best way. You can make better lines that look like centermarks if you wish, but lines is just faster.

See the reply in context

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EWP2 01 04-0.SLDPRT.zip560.9 KB

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Denny Metcalf Nov 30, 2011 4:32 PM
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Hi Reeshi,

I'm a little confused by your statement "if I make holes on flat pattern at equal distance, it won't match to the holes on cylinder," is the cylinder of constant radius?
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reeshi pradhan @ Denny Metcalf on Nov 30, 2011 4:38 PM
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If I punch the multiple holes on flat sheet before rolling it at equal sepatation using linear pattern, it will no longer equally distribute once it rolled/ bent.
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Denny Metcalf @ reeshi pradhan on Nov 30, 2011 4:53 PM
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Why would they not be of equal separation with a linear pattern (if a constant radius exists)?

There's many, many different ways to do this but lets try a fun approach:

--

Create a plane tangent to the sheet metal:

Set up your hole pattern:

Wrap the sketch to the face of the sheet metal:

Finished product:

It is up to you to fill in the correct dimension values though because you have not explained your cylinder.

If you know the radial spacing of the holes in the cylinder, you should be able to do some math to get what the linear pattern spacing should be (again, for constant radius). If you are off then I implore you to consider that perhaps you are not taking into account the thickness of the sheet metal or any gaps that you have included. It should work though, if you want, give me the numbers and I'll calculate it for you.
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John Stoltzfus Dec 1, 2011 7:43 AM
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Good morning Reeshi,

Do you have 2012 SW???

Later,

John
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John Stoltzfus @ Denny Metcalf on Dec 1, 2011 7:47 AM
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Good morning Denny,

An interesting and different way that I will try out later. I prefer to work with the hole cut position being related to degree patterns, but I'm going to try your way,

Later,

John
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reeshi pradhan @ John Stoltzfus on Dec 1, 2011 9:16 AM
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Good morning John,

I have solidworks 2010 only.

Reeshi
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reeshi pradhan @ Denny Metcalf on Dec 1, 2011 9:27 AM
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Hi Denny,

If you look at my model colsely from top, there is small lip coming out at one end which is giving me hard time.

My original model has everything all right where holes are made after rolling the sheet.
But in real practice or in 2d Drawing of sheet metal , we have to show and dimension the holes on flattern sheet.because we are making holes and then rolling the sheet, not first roll the sheet and make holes. Image below will gives you some sense how this sheet metal part going to be used. We use three piece of this part to cover complete cylinder.
.
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Casey Bergman Dec 1, 2011 9:38 AM
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Can you put in the first hole of the series on a tagent plane to the rolled surface and then use a circular pattern to drive the remainder of the series of holes? This is the approach that I would use.
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reeshi pradhan @ Casey Bergman on Dec 1, 2011 9:52 AM
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Hi Casey,
I did the same thing, but it can't be single part. It is composed of three parts rolled in 120 degree angle each and has over lapping lip too.
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John Stoltzfus @ reeshi pradhan on Dec 1, 2011 10:09 AM
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Good morning Reeshi,

Unfortunately I have 2012 so I can't show you how I would do this part, maybe I can explain.
1. I would have a part that is a dummy part, just full of sketches and I would setup the hole sketches in that part.
2. That part would be the first part in the feature manager tree.
3. Develop the new part using the dummy part
4. Use the Extrude Feature for the initial shape, rather than the Sheet Metal Bends
5. Add the Sheet Metal Bends after your part features are complete
6. Having parts that fit is the ultimate goal and if all of your part information comes from the same source fit is guaranteed.
After your part is complete you should be able to flatten the part and have it cut out with a laser or plasma and it will fit.

Later,

John

PS: I have 2004 on a computer at home, if you need me to do a sample for you let me know
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Denny Metcalf @ John Stoltzfus on Dec 1, 2011 10:25 AM
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Morning John

Radial dimensions are the design intent so for me also, that is the prefered method. However I wanted to investigate the OP's statement about linear patterns and wanted to just provide a different method.
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reeshi pradhan @ John Stoltzfus on Dec 1, 2011 10:32 AM
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Hi John,
Thank you for your suggestions. After flattern as in your process will those holes be dimensionable? I guess they wont be circular any more, right?
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John Stoltzfus @ reeshi pradhan on Dec 1, 2011 10:38 AM
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Good morning Reeshi,

You're on it,

The holes won't show up as a perfect circle and we're hoping that we will see Solidworks taking care of the Enhancement Requests that we need.

To get around this you need to make the first hole smaller and then in your flat pattern you need to add the true holes, to do that you will need another work around, by adding relation points or referenced geometry points.

I am not exactly sure, but within the last two months we did have a discussion on this and I can't remember what it would have been listed as.

Later,

John
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John Stoltzfus @ reeshi pradhan on Dec 1, 2011 10:44 AM
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Good morning Reeshi,

I did forget to mention that when you design a part like this you want the hole to show up round, so therefore you want the hole to be an ellipse shape when you cut the part, because the rolling of the part will distort the hole to a round shape, exactly where you want it. Otherwise you would need to make the part and then add the holes later and I'm sure that you understand that the holes won't be in the flat pattern.

These types of parts are more than meet the eye, right

Later,

John
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Denny Metcalf @ reeshi pradhan on Dec 1, 2011 11:20 AM
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Hi Reeshi,

Are you in the heat treating industry or something related?

Anyhow, a few years ago most of my work was holes through several layers of thin sheet metal so I had to try and come up with some clever methods to do this as quickly as possible. SolidWorks and Inventor were not near as nice to use then as they are now.

What I want to clarify is that the linear pattern will work for equally spaced holes in a constant radius and I think we can both agree on this statement. The spacing is going to be related to the angle by:

     r = Radius of Cylinder
     Θ = Angular Spacing of Holes
     π = Yummie Pi

Arc Length (of Cylinder) = (2 π r) * (Θ / 360°)

Assuming no gap between Sheetmetal Panel and Cylinder...

Arc Length (of Inside of Panel) = Arc Length (of Cylinder)

     t = Sheetmetal Panel Thickness

Arc Length (of Outside of Panel) = (2 π (r + t)) * (Θ / 360°)

     j = Jog Offset in Panel

Arc Length (of Outside of Panel with Jog) = (2 π (r + t + j)) * (Θ / 360°)

Keep in mind that these simple calculations work because we're using a Wrap, my wording here is just a bit misleading, lol.

The point here is that the linear spacing from hole to hole is going to be different in the area with the jog, but theoretically linear spacing will give equally spaced holes in a constant radius.
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Denny Metcalf @ reeshi pradhan on Dec 1, 2011 11:33 AM
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My suggestion is that you independantly calculate the location of the hole for the jogged area using math, it's going to be proportionate to the locations of the rest of the holes on the main part of the panel by a factor related to the jog offset.

Also, if at all possible try to position your panels (and holes) in such a way that all three can be identicle and you have only one part used three times. In other words, the number of holes should be equally spaced (as you said) and divisable by 3.

Alternatively, as John mentioned, you could just use a circular pattern and forget about all this math mumbo jumbo! Is this part going on a water jet / laser / plasma or is it getting punched?

If all you need are the coordinate values for the holes in the flat pattern, a circular pattern is perfectly fine because it won't matter that you're going to end up with a outside flat pattern that looks different than an inside flat pattern because the center points will be identicle.

If you are worried about splines, just clean up your geometry in your 2D editor of choice and replace with circles.
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John Stoltzfus @ Denny Metcalf on Dec 1, 2011 11:39 AM
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Good morning Denny,

"Good stuff"

With this assembly and having the wrap end up in three identical pieces will take some up front configuring and the way I would expand on what was already mulled over is this; My part would be viewed from the top and the hole development degrees and the part sketch would be determined from there.

Later,

John
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Denny Metcalf @ John Stoltzfus on Dec 1, 2011 12:12 PM
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Thanks John,

As I said in a previous example, there's many, many different ways to do this so here's another fun approach:

--

Start off with a dummy solid that is larger than the finished piece you want to make. Then create an extruded cut for your hole that will seed your circular pattern.

Make a circular pattern of the extruded cut, using the dummy cylinder as the axis of revolution.

Next, create the profile of the sheetmetal panel that you want. You can just sketch this on the top surface, it really doesn't matter.
Normally I would use some equations but I didn't want to spend too much time with this example. The important thing as that you follow all the sheetmetal rules like constant thickness, bend radius, etc.

Now extruded a new solid out of this sketch using these settings:
Can you see where I'm going with this yet? Oh, this is fun!

Now use the Combine feature and take the intersection, erm, common:

Enjoy the finished product:

--

Couple things to keep in mind, this approach works great and I use it a lot. I started doing this when I used Autodesk Inventor because of some software limitations, and to this very day it still works really well, though there are more elegant solutions. It's actaully a lot easier to do this in Inventor than it is in SolidWorks, but that's a whole different story.

Typically if you're going to use this approach, you should make your dummy solid into a part and then derive that part to make your panel out of it. I just wanted to get the point across quickly so I didn't bother with that because I didn't want to have to make more screenshots and explain why there's multiple parts going on.

If you're an equation junkie like I am, then you might appreciate this approach because it's very versatile.
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John Stoltzfus @ Denny Metcalf on Dec 1, 2011 12:16 PM
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Good afternoon Denny,

Again, Good Stuff, that is why we use SW in a way that is comfortable for "Me", right!!

The one part that I mess up once in a while is the, "design intent", which can change a lot when you design something. For me the biggest connection/correction tool that is needed when making changes is either a "Dummy Part" or a "Skeleton Part".

Later,

John
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Denny Metcalf @ reeshi pradhan on Dec 1, 2011 12:21 PM
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If you're really worried about it and don't like making dummy parts, configurations, cleaning up flat patterns, or having two different flat patterns depending on outside surface and inside surface...

Extrude tapered holes!

Seriously, it works, lol. Using some math you can come up with a draft angle for your holes so that when the part flattens out, the holes on the outside surface are the same as the holes on the inside surface.
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reeshi pradhan @ John Stoltzfus on Dec 1, 2011 3:17 PM
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Thank you every body for so many responses. Now I stuck in 2D drawing of this part. it is not letting me dimension the holes on flattern view.
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John Stoltzfus @ reeshi pradhan on Dec 1, 2011 3:21 PM
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Good afternoon Reeshi,

You need to add reference geometry points in the center of the holes and cut extrude a hole just a little larger so it comes out as a true hole, you need to do this in the part file so you can dimension in the drawing.

Later,

John
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Denny Metcalf @ reeshi pradhan on Dec 1, 2011 3:22 PM
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Hello Reeshi,

Could you please elaborate a bit what the problem is?
Which method did you use to model your sheet metal panels?
How did you export your flat pattern, did you export the face?

Is the problem that you ended up with splines?
Is the problem that you don't have center points?

John and I are both very willing to provide help but I think we need more to work with.
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reeshi pradhan Dec 1, 2011 4:54 PM
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Hi John and Denny,

Sorry for bothering you. I have no idea where I missed the thing. May be because of lack of manufacturing knowledge.
I think, I need 2D flatern view of rolled sheet for manufacturer, So I want to create 2D drawing out of sheet metal part file.
Which ever method I use to create sheet metal part with round hole, once I create 2D flatern view those holes no longer round and un-dimensionable.

John: how do I create reference point? I have created reference point and axis for each hole as in attached file, but once you flatern the part they are no longer use.
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- cover3.SLDPRT.zip387.5 KB
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Jeremiah Feist @ reeshi pradhan on Dec 1, 2011 5:14 PM
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make the reference point in the flat config.
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punched/Drill holes on rolled sheet metal

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