weldment profiles

Does anybody have some steel angle & channel weldment profiles they
would like to share?

I don't know why SW would introduce this functionality with no
library!
Maybe they will update with the next release?

Thanks,
Bob

 

I can send you our bulk material templates, but I looked at some of the
weldment documentation and it looks like you have to have an individual file
for each shape. Is this correct? If so, too bad, because we have all of
the channel shapes, for example, defined in a single part file as
configurations. It looks like for us to have all of those available for
weldments, we would have to break them all out. Comments? We haven't used
the weldment feature yet, so maybe I'm just missing something.

WT

 

profiles are nothing more than library features and need to be individual
files (.sldlfp)

 

Maybe I'm missing something, but there is under the toolbox menu the
'structural steel' dialogue that contains standard steel profiles?

Zander

 

yep, that's true. but you have to have toolbox (it's an option $$$).

 

Are you refering to 'No libraries' as not have any or the pathically small
library that comes with SW....??

 

i'm referring to "library features".

for weldments, profiles are created from library features.
for toolbox, parts are created via different configs (sketch is driven by
equations).

you could use a toolbox part to create "library features" for weldments.

 

Wayne,
Weldment profiles are individual Library Features so you will need to
convert every config of your part libraries. I have attached a macro that
will do this. Please note that this macro requires that you Save each part
to a template first - the macro will then run thru the part template and
convert each config to a separate Library Feature. MACRO WAS CREATED BY MY
VAR - SHANE PARKER OF INTERCAD - THANKS!! It has one problem - each
configuration that it creates makes it incrementally larger than it's
predecessor (e.g. on a 900+ config pipe the config was about 250 KB and the
last 6500KB) - I believe that Shane fixed this but I don't have a copy of
the updated macro. Maybe someone out there can give it a bit of a tweak to
reduce the file sizes.

To make your weldment profiles 'Smart' you need to add the custom properties
at the CUSTOM tab and NOT the Configuration tab and if you make these
properties parametric (i.e. linked to the part dimensions) they will auto
populate your cut list properties. e.g. I use Description (75x50 RHS) &
Material (not parametric) - the weldment function will auto create the
Length property for the cut length.

Also make sure that you put lots of 'connection points' on your part
sketch - e.g. on a pipe put a point at each quadrant.

It is also very important the you create the correct directory structure or
SW will not display them correctly (it needs to display 2 directories then
the size).
E.g. Hot Rolled Section/Equal Angle/

HTH

Merry

'
****************************************************************************
**
' C:\DOCUME~1\Shane\LOCALS~1\Temp\swx568\Macro1.swb - macro recorded on
08/27/03 by Shane
'
****************************************************************************
**
Sub main()

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim longstatus As Long
Dim longwarnings As Long
Dim boolstatus As Boolean

Dim FullPath As String
Dim PathOnly As String
Dim vPath As Variant
Dim TemplateName As String
Dim vTemplateName As Variant
Dim NameOnly As String
Dim ConfigName As String
Dim ConfigList As Variant
Dim ThisConfig As Variant
Dim Skname As String

Set swApp = Application.SldWorks

UserForm1.CommonDialog1.Filter = "*.prtdot|*.prtdot"
UserForm1.CommonDialog1.ShowOpen
FullPath = UserForm1.CommonDialog1.FileName
vPath = Split(FullPath, "\")
TemplateName = vPath(UBound(vPath))
PathOnly = Left(FullPath, Len(FullPath) - Len(TemplateName))
vTemplateName = Split(TemplateName, ".")
NameOnly = vTemplateName(0)

Set Part = swApp.OpenDoc6(FullPath, 1, 0, "", longstatus, longwarnings)
Part.SaveAs2 PathOnly + NameOnly + ".sldprt", 0, False,
Falseyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyy
Skname = InputBox("Sketch Name: ", "Name of sketch to use in lib
feature", "Sketch1")
ConfigList = Part.GetConfigurationNames

For Each ThisConfig In ConfigList
ConfigName = ThisConfig

Part.ShowConfiguration2 ConfigName

boolstatus = Part.Extension.SelectByID(Skname, "SKETCH", 0, 0, 0,
False, 0, Nothing)

Part.SaveAs2 PathOnly + ConfigName + ".SLDLFP", 0, True, False

Set Part = swApp.OpenDoc6(FullPath, 1, 0, "", longstatus,
longwarnings)
Next ThisConfig

End Sub

 

Hi Wayne, Bob, Merry, etal,

Do this,

Open a library file that has many configs in it. Named it, "Size"

Make sure the library file is saved in the proper location such as:

C:\Program Files\SolidWorks\data\weldment profiles\ansi inch\square
tube\size.sldlfp

Return to the size.sldlfp and change to the config you want as a weldment
profile and SAVE it but do not close it.

Open a new part file, create the profile sketch, close sketch

Insert a weldment, structural member,

Standard = ansi inch
Type = Square tube
Size = Size
Pick your path segment

Then walaa, you have the profile that was LAST SAVED in your multi
config-single file!

Go back to your size.sldlfp and change the config and SAVE the file.

Start another structural member do same steps above and the profile will be
the LAST saved profile in the "Size.sldlfp" file.

That's the work around I found to NOT having save a whole bunch of library
files...

I hope this helps,

Dan B.