Multi-Surface-Sheet Metal-Tank Repad-Complex Geometry Question

[jeanchile]

Hello all,

Thank you for taking the time to review this. I appreciate any suggestions the smart people on this forum can offer.

I have a de-gassing tank that I am working on that has a cone roof (steel plate construction). Through this cone roof is a square opening for an inspection hatch that is "flat to the world". This inspection hatch requires reinforcement around the opening in the form of a steel plate. Here is a picture of what the shape of the reinforcing plate will look like when complete:

I figured I would send this surface to sheet metal (or re-create it), thicken it, and flatten it out for the CNC table. The issue is, that leaves no easy way for the shop to form it into it's cone shape. The shop wants me to give them a flat pattern for a cone shape that encompases the repad with the outline of the square reinforcing pad "stitched into it". That way they will form the cone shape with small stitched cuts into it, then "complete" the cuts with a gas torch after it is formed and scrap the outside excess material. Like this:

On other similar parts I would usually just create the cuts/openings I need and then turn them into "stitches" in the CNC file using AutoCAD, but I can't figure out a way to do that when I have two cuts and three separate bodies (the inside scrap piece, the outside scrap piece, and the repad).

I originally thought about using a multi-solid, sheet-metal, table-driven, iPart to control the suppression of the different solids but then I remembered that sheet metal parts don't support multiple solid bodies.

I'm kind of at a loss at what to try next. The end result needs to be a completed formed model (which I have) and a "stitched", cone-shaped, flat pattern (which I don't have). Any ideas?

[jeanchile]

I keep coming back to a surface that is split into 3 seperate sections that I can thicken and flatten together but still maintain all the lines for the cuts. I just can't think of a way to make this happen: Something like this:

[jeanchile]

Also, Sketch3 in the part I attached above is the sketch I was using to control all of the geometry. The black sketch lines represent the extents of the cone section, the red lines the extents of the repad. This was all done in plan view because my intent was to trim a surface and thicken that surface. This method may not work now. This part started out as my idea on how to create the finished piece. Once I got stuck on the "means and methods" of creating it, it became sort of a mess. Once I've nailed down the best way to accomplish the task I'll likely start over with the part to clean up any of the un-needed work geometry, sketches, etc.

I imagine this gives more than enough information but if I've missed something, or been unclear, give me a holler.

[jeanchile]

Okay so I tried splitting the cone surface in the part I attached, then thickened the three sections I wanted, used Make Components to push that thickened solid out to a sheet metal part and got a flat pattern.

But... when I export the flat pattern to a ".dwg" to send to the CNC table I only get the outside profile:

Then I tried "Export Face" individually on each face thinking that I could maybe just insert the one face on top of the other as a block in AutoCAD but they didn't line up.

I am officially out of ideas and leave this in the capable hands of the forum. Thank you in advance for your help.

[Mario428]

2014 file done in sheet metal, change to suit as required.

Going by the proposed method of construction accuracy is not really on the table as an issue. LOL

I cannot help myself and must comment on how insanely complicated some of you can make a part, took me 10 minutes to do that.

[WHolzwarth]

Well, if a torch is used in the end, precision doesn't matter too much.

I'd do it this way.

Walter

[jeanchile]

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@Mario428 wrote:

2014 file done in sheet metal, change to suit as required.

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I can't. I'm on 2013 still. I appreciate the help and if you can, would you please post some screenshots including the Browser Bar.

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@Mario428 wrote:

Going by the proposed method of construction accuracy is not really on the table as an issue. LOL

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That depends upon how you define "accuracy". This is an API 650 tank fabricated by a steel fabrication shop using the usual API/AISC tolerances.

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@Mario428 wrote:

I cannot help myself and must comment on how insanely complicated some of you can make a part, took me 10 minutes to do that.

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I can't tell if this is a joke, a dig, or if you just missed what was said in my earlier posts (clearly you missed the file version). The file I attached was originally part of a larger multi-body solid file that was going to have the solids pushed out for the hatch sides, the repad, the gasket, the lid, the handle, etc. All of the parameters and some of the geometry are driven by another part file that is driven by other software and I removed the dependency so it was easier to post here. And for the record, creating that file took me 6 minutes according to our time tracking software so I win.

[jeanchile]

Thank you for spending some time with this Walter. Although your solution is not exactly what the shop has requested it has given me an idea on something to try. The shop has specifically asked for +/- 2 inch alternating stitches and that I leave the corner material un-touched. They only want to use the cutting torch for the small pieces in between the CNC cutouts and the corners.

Thanks for the help and I look forward to attempting a solution based on yours tomorrow.

[Mario428]

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@jeanchile wrote:

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@Mario428 wrote:

2014 file done in sheet metal, change to suit as required.

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I can't. I'm on 2013 still. I appreciate the help and if you can, would you please post some screenshots including the Browser Bar.

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@Mario428 wrote:

Going by the proposed method of construction accuracy is not really on the table as an issue. LOL

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That depends upon how you define "accuracy". This is an API 650 tank fabricated by a steel fabrication shop using the usual API/AISC tolerances.

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@Mario428 wrote:

I cannot help myself and must comment on how insanely complicated some of you can make a part, took me 10 minutes to do that.

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I can't tell if this is a joke, a dig, or if you just missed what was said in my earlier posts (clearly you missed the file version). The file I attached was originally part of a larger multi-body solid file that was going to have the solids pushed out for the hatch sides, the repad, the gasket, the lid, the handle, etc. All of the parameters and some of the geometry are driven by another part file that is driven by other software and I removed the dependency so it was easier to post here. And for the record, creating that file took me 6 minutes according to our time tracking software so I win.

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Yes you win, will go shopping and get a ribbon for the next time I see you. But what part of it only took 6 minutes, I saw a lot of discussion about complicated ways to make a simple part. I started from scratch but the ribbon is yours. LOL

I only have 2014 and we all know there is no saving backwards.

See attached screenshot

[jeanchile]

If there is anyone out there still willing to take a crack at this I am still looking for a viable solution. What I am trying to accomplish (other that what is stated above) is this:

1.) Have the part modeled that matches the method of fabrication (part of our software training 6 years ago).

2.) Obtain a flat pattern that is matches the way this part will be cut (all cuts normal to the material face).

3.) Have alternating 2 inch stitches that leave the corner materials.

----optional----

4.) Have one part that represents the full process from flat pattern burning to cone forming to torch cutting of finished part where I can show the process on a drawing.

Anyone have a way to do this?

Also, I don't think this matters to the solution but our actual process uses different software to engineer the entire tank, then we export design values, thenimport the design values to a master Inventor skeleton file, then derive (or link) the IV skeleton parameters to all of the parts as needed.

[Mario428]

Have attached my part as a stp file since you are on 2013,evidently stp files are not allowed

email me at    mario   at   cmpequipment.com and I will send it to you if it might help

[jeanchile]

Thank you Mario but a step file won't be necessary. I could see everything I needed from your browser screenshot. For the record though, if you zip the step file you should be able to attach it here afterward.

As it stands right now I have everything I need to complete the process except for the fourth "optional" step I listed above. It would have been nice to have this all as one file but I can deal with two (derived sketches driving both). This would be the first time I have not been able to get Inventor to match the manufacturing process exactly and it kind of bugs me though.

Thanks for the help.

[WHolzwarth]

Look at this. I think, it's rather close to what you want. I've unfolded the cone, projected your lines back to the unfolded sheet and used them as construction lines for the 2 inch pattern.

Problem is, that caused by unrolling your sketch lines, they are no more straight and rectangular. You can see it by looking at the slightly changed position of the 2nd column of torch cutouts. Therefore I'd use them only as construction lines, and create an exact rectangular cutout and pattern in unfolded situation. The differences are minor, and I don't think, that anyone can notice them in the end.

Walter

[Mario428]

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@jeanchile wrote:

If there is anyone out there still willing to take a crack at this I am still looking for a viable solution. What I am trying to accomplish (other that what is stated above) is this:

1.) Have the part modeled that matches the method of fabrication (part of our software training 6 years ago).

2.) Obtain a flat pattern that is matches the way this part will be cut (all cuts normal to the material face).

3.) Have alternating 2 inch stitches that leave the corner materials.

----optional----

4.) Have one part that represents the full process from flat pattern burning to cone forming to torch cutting of finished part where I can show the process on a drawing.

Anyone have a way to do this?

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This " 2.) Obtain a flat pattern that is matches the way this part will be cut (all cuts normal to the material face). "

My method does not give this because my cut is from the one of the planes uses for the lofted flange. But I would simply edit the flat pattern to make a normal cut. Project the lines that would give me clearance for the part that goes thru the cone and make a cut on the flat pattern only. This would give a clean part to your cutting machine.

Maybe I am missing something else in yuour process. The lofted flange can be done from a skeleton part quite easily.