Mitered 90degree sheet metal elbow 1

[jrings]

I would love to be able to do this in Solidworks. I am sure it could do it just haven't had the time. we currently use Sigmanest Develop to do these flat layouts for us and they work pretty well. Anyone else ever done a mitered elbow in Solidworks sheetmetal?

Joe Rings CSWA

 

[ctopher]

Can you please show a pic?
I'm not familiar with Sigmanest Develop.
Anything here help?

http://www.sheetmetaldesign.com/Cad-SolidWorks/index.htm

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Apr 30, 2008)

 

[jrings]

in sheetmetal to make a 90degree turn in ductwork you need to piece different segments of rolled steel together to make a 90degree turn

see link for an example.

http://www.indelco.com/c-2345-pvc-fabricated-3-piece-90-elbow--soc.aspx

Joe Rings CSWA

 

[ctopher]

The link I show above has a couple of similar examples that can be used. Attach each piece within an assembly.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Apr 30, 2008)

 

[CADGemini]

Since you will need to weld these together anyways I would lean toward using the weldment feature SolidWorks has. You basically sketch the center profile and create the profile of the tubing to follow. It is very similar to a sweep but allows you to select the type of intersections you want at each transition.

Using weldment will also give you the exact lengths and angle cuts needed for each section.

Hope this helps....

Best Regards,
Jon Knabenschuh

Gemini CAD Solutions

http://www.geminicadworks.com

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

Solidworks 2007

 

[CorBlimeyLimey]

Jon,
Can flattenable sheet metal parts be used in a weldment?

 

[ShaggyPE]

Can flattenable sheet metal parts be used in a weldment?

My recollection is no. You can have only one body in a sheetmetal part.

-Dustin
Professional Engineer
Certified SolidWorks Professional

 

[DanielGraham]

You can have a single sheetmetal part that you can flatten in a weldment if you like. I would probably suggest making a top down assembly though instead for most cases.

Daniel Graham

http://www.3dvision.com

 

[kp5054]

Hey Joe,
If you create a "tube" using the "revolved boss/base" (only revolving 359.5°)then create a sketch with your "miter". Use the "insert bends" command. Now it will unfold.
Is this what your looking for?


Ken

 

[ctopher]

I found this on the web.

http://litio-3d-sheet-metal-unfolding-software.download-702-14585.datapicks.com/

When I get the chance I will try it out.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Apr 30, 2008)

 

[jrings]

Believe it or not I have still not found a way to make use of Solidworks at all when it comes to duct work and transitions. I have given up on the elbow and now I can't even seem to get a simple offset round duct to work. I am pretty sure Solidworks was not the right software for our company.

Joe Rings CSWA

 

[DesignerGuy16]

If you model the 3 piece adjustable elbow into a flexible assembly and insert that flexible assembly into another assembly just make sure one end of the duct is fixed with mates. Then mate your next duct piece to the other end of the flexible duct. Then using distance mates you can lock down the direction and location of the exiting duct while having the flexible duct auto-solve.

Note it may take moving the assembly "close" to get the mates to stick without errors, but it can work. I've done similar, just not ducting.

Forget doing this in a weldment, make it's own assembly.

James Spisich
Design Engineer, CSWP

 

[tjohns]

Hi jrings,

We are creating 90 degree mitered elbows for our fabrication shop with Solidworks. Our company is one of the largest metal fabrication shops in the United States. We send all of our plates to Sigmanest for our cutting needs and we use the sheetmetal function to create those plates.

I don't think the weldment way of creating an elbow is the best way. I'm kind of confused how the sheet metal function would work as a weldment.

In any case the fastest way to create the elbow that you want is to create an assembly. Create a 2D sketch as a part. In that 2D sketch you want to draw your outline of the elbow you wish to create. Include your radius, centerlines, # of segments and your O.d of the elbow. Now insert the 2D sketch into your assembly. Start creating the elbow segments as rolled sheetmetal extrusions. Insert the elbow segments as parts into your assembly and mate into place. Now use the 2D sketch that you created as the driving sketch for your mitered cuts.

Assuming you want the best way to do it which isn't the fastest. Create your sheetmetal elbow segments within the assembly use reference planes and the 2D sketch to drive your entire assembly. This way you won't have to worry about mates if your assembly is created within context. The cool part is that if you go this route you have an assembly that can be used many times over and can be customized for different duct o.d.'s.

I know it sounds complicated and trust me the first time I tried creating it on my own without a starting point I almost gave up in frustration. My senior designer showed me the way our company created these mitered sheet metal elbows in Solidworks and it blew my mind how easy it was. This is an assembly that can be created in 5-10 minutes easy with only a couple of steps.

We've used this method for everything from 36" to over 14' O.D. duct.

p.s. quick tip make sure your weld seams don't line up when you create your mitered elbow segments. Can't tell you how much it sucks having to fix that simple mistake.


Tristan Johns
Lortz Manufacturing
Certified SolidWorks Professional

http://www.lortz.com