SolidEdge Can: Will SolidWorks do this????? 3

[Baroche]

Hello All

Please I am converting to SW from SE. How can I create this type of cutout in a SW sheetmetal part-(Notice the bent flange around the cutout).
Here:

http://home.comcast.net/~mamechi/CAD/SteelJoist.jpg

SolidEdge uses one command "Drawn Hole" under the "Dimple" feature in the Sheet metal environment.

Please what is the SW equivalent?

Thanks for any assistance

BTW: is it possible to get Solidworks to dimension the distance between two parallel planes. Can't seem to place this dimension. Could not place the dimension in a sketch and not in 3D sketch - What gives???

 

[smcadman]

Solidworks can do that as a drag-n-drop tool on a sheet metal part, but can't flatten it. Design library > forming tools > extruded flanges. See screenshot:

http://www.paul-flores.com/solidworks_screenshots/Extruded_Flanges.jpg

SW07 SP2.0

Flores

 

[AnnaWood]

If you are using SolidWorks 2007 you can use the sheet metal Edge-Flange command. This is new functionality that was added in SW07 to be able to add an edge flange to a curved edge. You may have to play with the settings and/or the edges you select a bit to get what you are looking for.

If in an earlier version of SolidWorks you will have to add non-sheet metal features to create the flange. You will also not be able to flatten the part.

http://www.acrodesigns.com/SolidWorks/Edge-Flange.jpg

Regards,

Anna Wood
SW06 SP5 x64, WinXP x64
Dell Precision 380, Pentium D940, 4 Gigs RAM, FX3450
WD Raptors, 1 Gb network connection

http://designsmarter.typepad.com/solidmuse

 

[AnnaWood]

Here is a link to the SolidWorks 07 file.

http://www.acrodesigns.com/SolidWorks/Edge-Flange.sldprt

Regards,

Anna Wood
SW06 SP5 x64, WinXP x64
Dell Precision 380, Pentium D940, 4 Gigs RAM, FX3450
WD Raptors, 1 Gb network connection

http://designsmarter.typepad.com/solidmuse

 

[AnnaWood]

By the way, to be clear, the Edge-Flange feature can be flattened in SW07.

http://www.acrodesigns.com/SolidWorks/Edge-Flange_Flattened.jpg

Regards,

Anna

 

[smcadman]

Nice one Anna, completely forgot about that tool. Is the flat pattern accurate, or do you to have fudge it a little? SW can do flat patterns of straight flanges perfectly, but square-to-round flat patterns can't be used without creative thinking.

SW07 SP2.0

Flores

 

[CorBlimeyLimey]

BTW: is it possible to get Solidworks to dimension the distance between two parallel planes. Can't seem to place this dimension. Could not place the dimension in a sketch and not in 3D sketch - What gives???

Are you wanting to do this in a model or a drawing?

If in a model ... Why? Offsetting a plane creates a behind-the-scenes dimension which can be accessed by double-clicking or editing the plane feature in the FM tree.

However if you really need to, don't create a separate sketch, just add a dimension from the Annotations or Dimensions toolbar by selecting the two planes in the graphics area ... for both model or drawing. Take note though that this will be a reference (driven) dimension, NOT a driving dimension .

 

[Baroche]

Thank you all for all your help. You guys are the best!

Regards

Michael

 

[AnnaWood]

No, the flat pattern is not correct. It does not account for the compression and stretching you will get going around the curves.

Still need a higher end add-on like BlankWorks for that kind of blank development.

It will get you a starting point, then you can add or subtract material with additional features to get your final blank.

Regards,

Anna Wood
SW06 SP5 x64, WinXP x64
Dell Precision 380, Pentium D940, 4 Gigs RAM, FX3450
WD Raptors, 1 Gb network connection

http://designsmarter.typepad.com/solidmuse