topic Re: creating pipe flat pattern in Fusion Design, Validate & Document Forum

creating pipe flat pattern

davidSWEUU — Tue, 20 Jul 2021 22:00:55 GMT

I am designing a stove pipe section that has multiple segments and grows at one end. I have it sketched, but when I try to create bodies, they don't create as sheet metal parts and therefore I cannot open them. Also, the create a weird bow instead of having straight edges. I did add "slices" so that they are not a closed body without a seem. The best I could figure was to use the sweep function. any other ideas or tools I should try?

Re: creating pipe flat pattern

jhackney1972 — Tue, 20 Jul 2021 22:42:29 GMT

I have not looked at your model but I am attaching a 5-piece sheet metal elbow that may give you some hints. It is parametric so you can change the size, within reason, if desired.

Re: creating pipe flat pattern

jhackney1972 — Wed, 21 Jul 2021 01:29:42 GMT

I tried to determine some general dimensions from your model but I am sure I missed them. I wanted to show you the general method of layout using construction planes and sheet metal contour flanges. In the first sketch I declared the split gap to be 0.5 degrees which can be changed within reason. I also did not bother with the one shorted side, that is simple to change by changing the length of the contour flange on one side and splitting the opposite side to make it shorter. By the way, I created only sheet metal bodies so you can only have one flat pattern at a time. If you want multiple flat patterns either redo the model using sheet metal components or maybe use the method outlined in this blog article and video. Model is attached. If you need an explanation of how it was done, just follow the timeline.

Re: creating pipe flat pattern

jhackney1972 — Wed, 21 Jul 2021 02:33:47 GMT

I need to make sure that you understand, using the method shown in my model, the edges of the developed flat pattern(s) will not be square, they will be slightly beveled. This can be eliminated but for this example, I did not take the time to do this process.

Re: creating pipe flat pattern

davidSWEUU — Wed, 21 Jul 2021 05:59:20 GMT

Thank you. I have managed to get most of the way, but one section needs to transition from 7.625" to 6.625. this creates a weird transition and I am struggling on this one. I have followed some youtubes for square to rounds, but it did not work for me. when I try to convert to sheet metal, I can't seem to find an appropriate edge that it will accept for the conversion. I attached a cleaner file. Section in question is section #2

Re: creating pipe flat pattern

davidSWEUU — Wed, 21 Jul 2021 09:26:31 GMT

I have figured out all of the segments except the one that transitions from 7.625 to 6.625. I have made a body but cannot flat pattern it. i cannot figure out why. the component I am closest to is the test component.

Re: creating pipe flat pattern

TheCADWhisperer — Wed, 21 Jul 2021 12:00:06 GMT

Your Sketch1 is not fully defined. (The very foundation of your design.)

I would start there.

There are repeated dimensions - generally not needed.

Many white dots (not good).

At least one duplicate line overtop of identical line...

An unresolved issue highlighted in the Timeline...

All Gores must have at least a microscopic planar flange.

I would use only Revolves (no Lofts) for this design (and Extrude or Sweep for the previously mentioned planar flanges).

Although Loft can return cylindrical, conic and planar geometry - it is generally best to use the most primitive geometry definitions possible.

As I try to decipher the true Design Intent - I have to wonder where this dimension came from?

I would expect this to be the controlling dimension?

Re: creating pipe flat pattern

TheCADWhisperer — Wed, 21 Jul 2021 12:28:21 GMT

My Sketch1 comes out like this - although I am a bit concerned about where 4 of the dimensions came from.

I generally use only dimensions that I can easily measure out on the shop floor.

Four of these Gores are simple trimmed cylinders while one is a trimmed cone.

Once the dimensions have been verified - I can proceed with the sheet metal parts.

Re: creating pipe flat pattern

jhackney1972 — Wed, 21 Jul 2021 14:13:10 GMT

One thing that will help the forum users, you need to click on the responder post YOU ARE REPLYING to. You are replying to yourself so no one, at least I do not, know how to respond.

Re: creating pipe flat pattern

davidSWEUU — Wed, 21 Jul 2021 18:59:04 GMT

Thank you everyone. I spent a bunch of time working through my sketch and cleaning it up. I was able to get a working part, but it wasn't perfect, much to my dismay. because cutting round pipe on an angle creates an ellipse, I struggled to get the same profile. I was able to get close enough for my purposes. This is the reason I was veering towards a loft. it made a nice clean ellipse, exactly as I needed. I will need to spend more time with it for my own learning, but it sounds like loft is not going to work for me, if I understand what has been said here.

Re: creating pipe flat pattern

davidSWEUU — Wed, 21 Jul 2021 20:40:06 GMT

Thank you,

The 7.701 dimension should be 7.625. And overall dimension should be 21.75 on the inside of the material. the rest look good. I am hoping you can help here.

Thanks!

Re: creating pipe flat pattern

TheCADWhisperer — Wed, 21 Jul 2021 21:22:00 GMT

@davidSWEUU wrote:
And overall dimension should be 21.75 on the inside of the material.

I don’t know what this means?

Why didn’t you simply edit the sketch and then Attach the corrected file here?

Re: creating pipe flat pattern

davidSWEUU — Wed, 21 Jul 2021 21:42:32 GMT

You are right, I'm sorry. Thanks again for your help. here is the updated file.

Re: creating pipe flat pattern

TheCADWhisperer — Wed, 21 Jul 2021 22:42:00 GMT

@davidSWEUU wrote:
And overall dimension should be 21.75 on the inside of the material.

Previously I responded that I did not know what you meant by this.

Your latest file does not have the 21.75 dimension on the sketch, so I had to go fishing.

This is what I caught.

Now I can proceed to fry it up...

Re: creating pipe flat pattern

TheCADWhisperer — Thu, 22 Jul 2021 17:46:59 GMT

Well, after a bit more experimenting I realized that you would need Autodesk Inventor Professional for that one Gore.

Re: creating pipe flat pattern

carl.j.barker — Fri, 23 Jul 2021 14:52:03 GMT

Not entirely sure I followed this thread correctly. but anyway how's this ?

Re: creating pipe flat pattern

TheCADWhisperer — Fri, 23 Jul 2021 16:43:04 GMT

@carl.j.barker wrote:
... but anyway how's this?

Model the two parts on either side of that one and take a look at the seams with the other two parts.

What do you observe? (Don't look below.)

For sheet metal - might be close enough with a bit of tinkering, but I don't know.

Re: creating pipe flat pattern

davidSWEUU — Fri, 23 Jul 2021 17:48:35 GMT

Thanks for the attempt. Yes, cutting a circular pipe on a mitre gives an elliptical face. Same with the cone, but because of its structure, the ellipses don't match. It requires advanced layout techniques. I may do it manually in fusion. Seems wierd, but if it allows me to CNC it..... And get the practice.

Re: creating pipe flat pattern

carl.j.barker — Fri, 23 Jul 2021 18:21:00 GMT

Ah yes I see the issue.

Creating the parts either side first and lofting appears to work.

Re: creating pipe flat pattern

TheCADWhisperer — Fri, 23 Jul 2021 18:29:25 GMT

Whoa, you got it to flatten.

I didn't even try.

Now you have me interested.