Need a Flat Pattern - Surface?

[DeSimulacra]

I have a model with a obround intersected by a cone. Being as it is Ti, I would like to create a flat pattern for the fabrication shop.
The large end of the cone lays against one of the flats of the obround but also intersects both of the end radius sections. I used the cavity feature and have a good 3D model. I don't believe that I can use the unflatten sheetmetal feature because of the bevels created (it has not worked yet). Is there some other way to get a flat pattern? Maybe using a surface? I can model the two features in question anyway possible, easily, if you have a method. They do not have to be an actual part of my assembly.
Hope this isn't clear as mudd.

 

[Theophilus]

You may need to clarify what the part looks like by posting some images (see FAQs for how to do so).

Meanwhile, you can probably build a sheetmetal part from the new part you have now--extrude a thin feature as a separate body within your part or within a new assembly--using your part's geometry as reference. Insert Bends, etc. to get the sheetmetal to form. From that, you can get a flat pattern. (See Sheetmetal in Help if you're not already familiar--lots to read.)


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[DeSimulacra]

Here is a test image

 

[DeSimulacra]

here is a sheet metal part that is what I need flattened

 

[Theophilus]

If that feature is truly conical, what I would do is create the conical part as a sheet metal part (insert bends, etc.). Use your oblong shape to cut the oblong shape out of the sheet metal part while it's folded. Flatten the bends to get the flat pattern.

Keep in mind where you want your seam when creating the sheet metal part.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[DeSimulacra]

Theophilus
Thx for the help. I wonder if you have any other ideas? Here is the error message I get.
"Flat-Pattern2: This bend has a cut that creates a beveled edge, which cannot be handled."

 

[DeSimulacra]

Is there anyway to create, edit in assembly and unfold a surface?

 

[alolesen]

If you get rid of the beveled edges this should work. I made a cone myself, the other day, and it worked fine.

 

[MElam]

In your cut feature, is the "Noraml cut" option checked?

 

[Theophilus]

Yeah, you're probably getting very thin edges where the rounds fade off from your oblong form. Think of it as true sheet metal and see if you can cut it a little better, since sheet metal will be sheared or punched without having razor edges like that.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[engAlright]

You can use a surface to create sheet metal - in this case your cone would be a lofted surface, you would then trim the surface to the face of the other part, then you thicken the surface to the thickness you want. You then "Insert Bends" to unbend the part. As long as the part has constant radii and is of a uniform thickenss (which it is guaranteed to be with a surface thicken) you should have no problems turning it in to sheet metal with insert bends. This method only causes problems when you have compound corners.

to ensure you have a constant radii on your surface, make sure your loft profiles have the same radii curves. Also, since your part is symmetrical you only have to do this process for one side, then mirror the finished "thickened surface" model.

 

[DeSimulacra]

Thx
engAlright I think your solution will work, if I understand you correctly I can create my cone as a surface and place it in an assembly, mated with the part I want to trim to. Then
'trim" the surface to the shape required, thicken the resultant surface, insert bends and unfold. ? ( I haven't worked with surfaces and this software)
MElam I tried that both ways, didn't work
Theo I realize the thin edges/bevel is my problem. I hope the solution engAlright gave will work. As solids the parts have no choice but to create these problems.

Thanks all for the input!!