CAN I CREATE A SOLID, SHELL IT & TURN IT INTO A 3 PIECE FLAT PATTERN?....?.OR DO IT ANOTHER WAY?

[Turbomist]

Hi there.......thanks in advance for any help. I have searched the tutorials and 'help' but have had no luck in finding an answer. I'm using SW version 2006.

I want to create a 3 piece flat pattern for the part I've attached. I'm not familiar with everything SW is capable of but I have had success in the past with other flat patterns.

I looked into the 'split' command...wasn't successful. Then I thought I might be able to start with the middle section (including the flat section on the top) as a sheet metal part and then create the side parts on assembly....but a 3D sketch on isn't available when creating on assembly.
Our company is presently getting by with a hand laid out pattern ....but there is a lot of trimming and filling going on.
Any help would be greatly appreciated.

 

[rollupswx]

First thing I notice is that there are no dimensions in Sketch1.
What happened to the dimensions?

Second thing I noticed is that Sketch1 is not placed with obvious symmetry about the origin.

Third thing I noticed is a fillet in Sketch1 that appears at one "bend" but not on the "symmetrical" geometry.

One technique would be to add the missing fillets for the bends.

Delete the faces rather than Shell.

Thicken the resulting surface bodies into the individual sheets.

 

[TheTick]

The problem is your CAPS-LOCK button. Pry it off the keyboard and get it as far away from your desk as possible.

 

[Turbomist]

thanks for your answer rollupswx.
The sketch wasn't defined because I had imported it from AutoCAD to give the idea of what I was trying to do.
I did delete the faces(leaving the side piece)but the problem was I couldn't turn it into a sheet metal part or flatten it. I really need the flat pattern but I just don't know how to get there.
Any other suggestions?
Thanks

 

[MikeHalloran]

I have on occasion modeled a part as a thin 3D solid, and then, sort of, managed to convert it into sheet metal.

When I was able to do that at all, an otherwise identical part that started out as sheet metal performed more logically in its interactions with other parts, and SW crashed less.

I.e., I infer that there is some internal conversion mechanism from solid to sheet metal, but the parts are somewhere somehow fundamentally different.

... as are real castings and real sheet metal parts, so I don't see the difference within SW as a huge problem.



Mike Halloran
Pembroke Pines, FL, USA

 

[drawoh]

Turbomist,

I routinely model blocks, hollow them out, and convert them to sheet metal.

Don't let SolidWorks do the ripping. Do it yourself.

--
JHG

 

[Turbomist]

DRAWOH Thanks, could you expand on the manual ripping please. If you see the attachment of the basic shape of my part in my first post, you'll see I would be trying to rip along an edge that is in multiple planes. I've tried converting the edge to an entity to make a cut but that doesn't work. I've tried a 3D sketch....couldn't get that to work.
I need a bit more of a step by step explanation if that's possible.
Thanks in advance.

 

[rollupswx]

This one is pretty easy.
First thing I did is "fix" the sketch as it appeared no real effort on getting it constrained. (I didn't change the dimensions.)

Then I offset the faces by zero.
Thickened them and converted to sheet metal.

 

[rollupswx]

I always expect to see effort on the basics.
In fact it takes no more time or difficulty to sketch correctly.

 

[rollupswx]

Top Flat Pattern

 

[rollupswx]

One of the 2 side Flat Patterns.
(I'm not sure if r2006 would allow multi-body sheet metal.)
If not, it is a simple process of doing one at a time.

 

[drawoh]

DRAWOH Thanks, could you expand on the manual ripping please. If you see the attachment of the basic shape of my part in my first post, you'll see I would be trying to rip along an edge that is in multiple planes. I've tried converting the edge to an entity to make a cut but that doesn't work. I've tried a 3D sketch....couldn't get that to work.
I need a bit more of a step by step explanation if that's possible.
Thanks in advance.

I do ripping as sketches and extruded cuts. Do you understand how your sheet metal part will be flattened out? Typically, I want this done my way.

Use the linked dimensions feature. Sheet metal creates the link "Thickness" to control all the wall thicknesses.

--
JHG

 

[Turbomist]

Thank you ROLLUPSWX for your in depth answer. I know how to define a sketch and I guess I can expect a telling off if I post an undefined sketch on a forum. My bad.
Unfortunately SW 2006 does not have the Convert-Solid capability. In version 2006 the way to convert to sheet metal is to rip and then insert bends.....this has worked for me on more regular shaped parts and gives a one piece pattern. If there is another way to slit the part into 3 parts, convert to sheet metal and unfold it, I haven't found it.
I think I might be SOL on this one.

 

[rollupswx]

Insert Bends should work just as well.
I often have to use this legacy tool rather than Convert-to-sheetmetal.