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Sheet Metal for curved part

ptc-4161478
1-Newbie

Sheet Metal for curved part

Hi all,

I'm trying to get sheetmetal drawing from part created with swept blend feature.

The trouble I'm having is to use edge rip tool to split the curve. The part I would like to make is attached here.

I have tried a simpler pyramid shape (square top square bot) and was successful in making the sheetmetal.

Thanks in advance for your help.


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1 ACCEPTED SOLUTION

Accepted Solutions

This was definitely a lot more work than I thought it would be, but it is possible.

Creo 2.0 attached

unbend_3.PNG

I used the merge from an assembly level to get the other 3 walls. I you open the assembly 1st, then open the contraction_2.prt.

However I don't know how you are going to form this in the way I modeled it. I could see this more like a clamshell design. Weld two edges along the bottom and 2 edges along the top.

View solution in original post

12 REPLIES 12

The only thing I could do was to do a surface rip on 3 of the faces (6 surfaces). After that, I was able to do an Unbend feature. I removed the small radius ont he top and removed the top surface in the shell command.

unbend.PNG

I was trying to printout the design and make it. But I guess i can merge multiple of the same design in photoshop. Unless anyone else found a way. Thanks Antonious, admirable problem solving skill you have.

Funny shapes in sheetmetal are not easy to deal with. If I wanted a flat pattern of something close to this, I would probably make this with surfaces and use Flatten Quilt to get an fairly accurate flat pattern for each wall.

You have to decide on how you want the edges to merge at the corners but this certainly possible within Creo.

Just because it -is- sheetmetal, doesn't mean you need the sheetmetal module to come up with the right geometry. I have done ribs that have a curved profile in two direction in core Creo where sheetmetal simply cannot do that. If you want a close representation to allow for bend allowances, when you thicken the quilt, offset it to both directions.

This was definitely a lot more work than I thought it would be, but it is possible.

Creo 2.0 attached

unbend_3.PNG

I used the merge from an assembly level to get the other 3 walls. I you open the assembly 1st, then open the contraction_2.prt.

However I don't know how you are going to form this in the way I modeled it. I could see this more like a clamshell design. Weld two edges along the bottom and 2 edges along the top.

View solution in original post

so the same surface rib approuch is required for complexed profiles like below, or it can be done more directly?Rolled+Sheet.JPG

TomD.inPDX
17-Peridot
(To:Dante)

I've seen this one done successfully with the sheet metal conversion tool. I've never had much luck with it though. You might search the forum for that one. Hopefully someone will help with a link if you have trouble finding it.

This is one made from 2 pieces that can be fabricated with the assumption of requiring seam welding.

unbend_4.PNG

I having difficulties openning both the zip files. I'm using Creo 1.0

Sorry, yes, I have Creo 2.0 so I cannot make one compatible with your version. But you should be able to do what I do. I will make a quick video of the features for you.

Please tell me which verion you need me to show.

I have done it following the first method presented. If you make a video it would be useful for others, so I guess doesnt matter which version. thanks

I am finding that the sheetmetal converter is very touchy at the small angle from the base. It works most consistently using surfaces and thickening afterward. this really is a challenging part.

People using Creo 2.0 can open the applied files. I will walk though the 2nd version in a video.

This is the video for this part. Please note the following:

1. The flatten quilt is only there as a comparison. I used to to know if the part had a snowballs chance of unfolding properly in Sheetmetal.

2. The part was a convention solid part converted to sheetmetal when the 1st wall feature shows up.

I will also offer a tip as to converting a sheetmetal part back to a solid. Move the "insert here" bar above the conversion feature (any sheetmetal feature) and you can easily regain all your original solid part features. Without moving the "insert here" bar, you might have the whole part roll up into a single feature.

Please feel free to ask questions. The attached Creo 2.0 file is what was included in the previous post. (contraction_a.zip)

Video Link : 4191

you tube link:

http://www.youtube.com/watch?v=rzyxBrQQNow

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