CONE??

[naresh843]

HI...
i am frustatd to get the result as customer needed...
1)i have a cone,which i need to split in to two parts as shown in image1...
2)After that i need to convert both parts individually into sheet metal.basically it is in surface,i need to thicken to 6mm..then to sheet metal,
3)Now finally i want to a flat pattern...when i convert it to sheet,by inserting bends it shows error

i can split the surface..but how i proceed further??

and also how can i project conical surface to a flat surface as shown in image2 (its like to project the half cone to a flat surface)..all this i can able to do in UG,but how in SW??

Thank in advance...

UG NX5,SOLID WORKS

 

[Eltron]

Why do you have to insert any bends in order to make it a sheet metal part?

Dan

http://www.eltronresearch.com

Dan's Blog

 

[acavite]

This question has been a rather frequent one in my brief time here. Might I recommend using the search feature prior to asking a question.

This thread should answer your question...

http://www.eng-tips.com/viewthread.cfm?qid=199521

 

[williedawg]

After perusing those earlier posts re cones, I experimented with the different methods of construction and was able to make cones using; 1)Lofted Bends, 2)Revolves, and 3)tapered extrusions using Polygon Sketches, ala Brake-bent parts.

Part of the "trick" to doing these is to make the cones a tad less than 360deg. You can then do a Suppress of the SheetMetal Bend, Insert a Plane onto either (what was) the external or internal cone Face, then make your Drawing using that view.
If you want 2 equal pieces for further processing, just insert a Plane after the Suppress and cut the part in half.
Remember to Suppress these Planes if reverting back to the cone model, otherwise there will be errors.

(Acutally, I think I downloaded someone's working model of the Polygon method, but can't remember who to thank for it.)

If you'd like to see the steps of the Revolve construction, I have some jpgs that I could post.
I'd upload the actual model, but I only have SW2006.
I could also show how the Lofted Bends and tapered extrusions were done if you're interested....again in jpgs.

 

[naresh843]

I would like to thank all,i got some idea after going through previous posts and other sites ,and williedawg if you can upload those swparts,it would be hepfull to me.i have sw2006 also..meanwhile i'll try to do with suggestions you posted..

Thanks in advance

UG NX5,SOLID WORKS

 

[rollupswx]

Whatever method you use make sure the cut edges are perpendicular to the flat. Go to the flat pattern and turn off shading and examine the edges from a perpendicular view. There should only be one line.

 

[williedawg]

Here's the Revolve method of constructing a Cone to apply SheetMetal bends to (I'm hoping, as this is my 1st try at linking to a file-saving site, so please bear with me..)

http://www.4shared.com/file/106445052/6af800e4/Cone_Revolve.html

 

[smcadman]

Sorry williedawg, but I'm sure the flat pattern is wrong. First off, I'm surprised SW let you use that part as a sheet metal considering one edge wasn't perpendicular to the face on one end.

That said, I dimensioned the flat pattern and the following just does not jive up with what it is supposed to be:

Large arc radius
Small arc radius
Large arc chord length

(The arc angle was correct for some reason)


Flores

 

[williedawg]

smcadman, thanks for the feedback.
I looked at the model and at first agreed with your comments, but kept looking at the sketches/dimensions in an attempt to see just what was going on.
I revised the sketch for the Revolve a little so that dimensions were easier to track. (also, I noticed the rectangle of the Sketch had a non-parallel short side at what would become the Large Arc; which was then corrected so that the Sketch is now a rectangle)
Note the Point in the Sketch which was used to construct a Circle of 4" dia; circ = 12.56637, and further, if we consider 359.75/360 as being the Revolve amount, we get 12.557644

When the SheetMetal feature was Inserted, one of the outer Edges was used for "Fixed Edge" and the K-factor set to .5
(The tighter the Bend, the more this ratio would need to be considered for change, but for a part such as this with a thickness of .0625 and proportionally large diameters, I just used the default.)

Given the basic dimension of 2.0000" to the Midpoint of the small end of the Revolve Sketch and the Revolve-Midpoint feature set to 359.75deg,
the Short Arc Length calculates to 12.557644
[2.0000*2*Pi*(359.75/360)] which agrees with the number based on the 4"dia stated above.

The Long-Arc Length (basic dim of 2.52094453radius) calculates to;
[2.52094453*2*Pi*(359.75/360)] = 15.8285619

All of these dimensions are figured at the "Neutral Sheet" (with K-factor = .5)

Here's the revised part.........

http://www.4shared.com/file/106484431/dfeed460/Cone_Revolve.html

 

[smcadman]

williedawg, below you will find an Excel workbook that I use to double-check the flat pattern.

Many times I make a second configuration, suppress the original cone, then make 2 arcs and lines (make a 2D flat pattern in other words). Finally I extrude them as a sheet metal part to save as a DXF for the laser. The downside is that it is a dumb part and does not update with the 3D model. The upside is that the flat pattern is correct, you just have to remember to update it.

Sheet metal workbook LINK



Flores