I’m having trouble trying to flatten a ‘pipe clamp half’ when it is a conical design. The important factor is to have the mating faces of the flanges in the correct location, 180 deg apart, or coincident with the front plane in my case. The attached part is modeled correctly but doesn’t flatten. I actually prefer doing a revolved thin part, insert bends, and add the flanges. But if you revolve 180 deg, the flanges add too much material due to ‘bend outside’ flange location. Changing revolve to 179 deg or so may actually work fine for this part, but I’ve had lots of cone parts that have too steep of a slope that the flange still interferes, or is not projecting parallel to front plane. Sorry for the boring Monday read… but does anyone have a better solution for this? Currently I manually (AutoCAD) subtract extra material in my flat pattern when laying out to lasercut.
Attachment – 2009_8_10_14_10
Tagged: sheet metal Toggle Comment Threads | Keyboard Shortcuts
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ivanl
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Doug
Hi again
How do I link a file to this forum. I would like to see others view and hows on a sheet metal part?
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admin
I am working on a button to do that but in the mean time if you hit ‘Edit Post’ on your posts you can add a file via the editor that comes up. Otherwise just add the URL
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Chris Serran
In my parts I add reference dimensions to show stock sizes, I then link those 3 dimensions to custom properties. In my drawing I reference this property for my stock size.
The issue I’m having is when I do this for sheet metal parts. I’ll flatten the part, put my dimensions on but when I unflatten the pattern the ref. dimensions change.
Unless I always keep the part flattend through configurations, the drawing will show the stock size of the part as if it were folded.
I’m trying to get away from manually typing in the stock size, does anyone have a workaround for this?-
CBL
When creating the dimension in the Flat, do not select an edge across which a bend is made. If possible select two vertices or two parallel edges representing the overall size of the part.
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Chris Serran
I run into problems when there is a bend on every side.
Flat:
http://screencast.com/t/Ub4oPfQ4Xd
Folded:
http://screencast.com/t/eN1CRyVpu -
Setsudo
I worked at this for a long time, the only workaround that works at all is to sketch your part in a top-of-tree layout. Then you can trace it in your sheetmetal base feature (do not convert entities, use coincidents) fold up your base feature and then dim the layout instead. Of course that will only work for something modelled flat and then folded up. If you want to do the reverse there is a way, but it is so convoluted I won’t go into it. Short answer is…it’s always less work just to type them in.
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CBL
Chris, I think you missed my point. The dimension can be placed across an area which has bends, but the dimension itself should not be created by using an edge which gets bent.
Select vertices or parallel edges instead.
http://img91.imageshack.us/img91/1372/vertexselectionpt9.png
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Chris Serran
Thanks Kelvin! The dimensions are dangling when folded but I can live with that.
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CBL
If the dimensions are placed on the Flat Pattern annotation view, they will not show up on any other annotation view, so the ‘dangling’ property will not be seen when folded. Having the correct dimension in the properties is the critical goal.
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Setsudo
Ooops, my method wouldn’t have any bend deduction… I just tried it, I’ve been doing wire that way though, since I have to calculate bends manually anyway.
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Adam_B
another option is to do a sketch on the flat pattern (aftet the flat pattern feature in the feature tree. Put your dimensions in that sketch. the Sketch will be supressed when you re-suppress the flat pattern, but the custom properties will still keep the correct dimension. A colleague seemed to think that you have to select the fixed face to sketch on rather than one that folds, but i’m not 100% that this is the case.
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ivanl and 
Adam_B, 
CBL, and 1 other are discussing. 
gupta9665 1:52 am on August 11, 2009 Permalink
Not sure why you designed it like this way. Simply create the 180° cone and then add edge flange. If you don’t know, you edit the profile of the flange by clicking on “Edit Flange Profile”. Look at the pic.
gupta9665 1:54 am on August 11, 2009 Permalink
Not sure why didn’t pic showed up.Attachment – edge-flange-profile
ivanl 2:16 pm on August 11, 2009 Permalink
I have made it like you said, but it only works well with a straight cylinder. On a steep cone the feature ‘works’ but doesn’t correctly lay it out. Insert it into assembly and do a circular pattern around a ‘mid axis’ and you’ll see the interference. Take the revolve back a degree or two and you’ll see a growing gap. The flange will no longer be parallel to the front plane.