Using a dimension of a part to pull a part into an assembly

  • Thread starter Thread starter Jeff
  • Start date Start date
J

Jeff

This is a bit of a long shot but here goes nothin... I am trying see if
it is possible to have solidworks look at a diameter dimension of a
round pocket in a part that is in an assembly, then go pull the
corresponding part out of a library that matches that diameter of the
part pocket... these diameters change depending on the stock object we
want to put into those pockets... I am trying to automate our design
some by using a VBA macro inside Excel to control the assembly... i can
make the assembly grow, shrink, do whateever i want, except the insert
the components for me part... If my above description doesn't make
sense, i will try to clarify... Any help you guys can give, would be
great... Thanks in advance...
 
Look at Smart Components - might be just exactly what you are looking for.
One example of the usage is to have a shaft of a given diameter, pull in a
snap ring that sizes itself to the size of the shaft, and then it in turn
puts the proper size groove in the shaft.

WT

Jeff said:
This is a bit of a long shot but here goes nothin... I am trying see if
it is possible to have solidworks look at a diameter dimension of a
round pocket in a part that is in an assembly, then go pull the
corresponding part out of a library that matches that diameter of the
part pocket... these diameters change depending on the stock object we
want to put into those pockets... I am trying to automate our design
some by using a VBA macro inside Excel to control the assembly... i can
make the assembly grow, shrink, do whateever i want, except the insert
the components for me part... If my above description doesn't make
sense, i will try to clarify... Any help you guys can give, would be
great... Thanks in advance...
Click to expand...


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As long as will you know the filename you want to insert, you can do
it. The way that pops into my mind would be to name the files in a
standard way (with the dimension in there). So maybe you have a
0.250-SHAFT.SLDPRT, 0.500-SHAFT.SLDPRT, 0.750-SHAFT.SLDPRT, and a
1.000-SHAFT.SLDPRT. Then if your dimension is X.XXX, you could concate
the filename such that the macro inserts X.XXX-SHAFT.SLDPRT. Or even
have some sort of lookup table that tells you for each dimension, which
file to insert. That would work fine too.

If you wanted SW to actually open those other files and measure
something there then close the file, and keep doing this over and over
until it found a matching dimesion...I'd guess you could do that too
but it'd probably be pretty slow. It'd be a lot faster to put that
value in as a file property because you can access those without
opening the files in SW.

Ken
 
Thanks guys for your help so far...

Ken, how do i go about setting up a macro that do the if dimension is
"x.xx" then the macro inserts x.xxx-shaft.sldprt... I am not having
much luck finding adequate examples to steal stuff out of :) Also, how
do you create a look up table? thats definitely what i am looking to
do, just dont know where to look or start to get my dreams to come
true... thanks again...

Jeff
 
You should check out DriveWorks to do what you want
(www.driveworks.co.uk). It's perfect for this kind of stuff.

However, assuming your model is not that complicated, I also think
configurations are the way to go. Maybe your excel macro could have a
lookup table that chooses the name of a configuration based on your
dimensional input?

You could still drive the dimension based on your spreadsheet (update a
specific dimension) but the configuration would control the "state" of
the parts and mates (supressed/unsuppressed)

As far as lookup tables are concerned, they're pretty easy once you do
one or two.

The common command for the lookup table is :

=VLOOKUP([lookup_value],[data_range],[return_column],[boolean])

What this function does is finds a value (lookup_value) in the leftmost
column of data_range. If it finds the value, it will return the value
of the cell in that row which is return_column number of columns away
from the first column.

I'll e-mail you an example.
 
I have tried the driveworks that came with 2006, seems to work pretty
good, just cant find good documentation and tutorials... the VLOOKUP
looks like a viable option... I get want it does, but i cant figure out
what code to put in the cell that is recalled by the vlookup so that it
goes and gets the part or assembly i am looking for.... i am making my
head hurt thinking about this stuff, and its a friday, i must be
sick... any additional help or pointers would be great... thanks
again...

Jeff
 
Kinda hard to tell you waht to do without knowing more about what
you're attempting to accomplish.

My thought was that you would populate the "data" field (for your
lookup) with configuration names, which would coorespond with the type
of data in the 2 dimensional array (for example, length x diameter).
Dunno?
 
Jeff,
I hope the below gets you a push in the right direction.
Ken

To Insert a component named MySlotWashers into the assembly:
Set MySWComponent = swApp.OpenDoc6(MySlotWashers, swDocPART,
swOpenDocOptions_Silent, "", fileerror, filewarning)
Set MySWAssembly = swApp.ActivateDoc2(MySWAssembly.GetPathName,
False, nErrors)
Set NewComponentID = MySWAssembly.AddComponent4(MySlotWashers,
MySlotWasherConfig, 0, 0, 0)

To Add a Coincident Mate:
'Coincident Mate
MySWAssembly.ClearSelection2 True
boolstatus = EntityArray(1).Select4(True, swSelData)
boolstatus = MySWAssembly.Extension.SelectByID("Bottom Mate Plane@"
& NewComponentID.Name2 & "@" & MySWAssemblyName, "PLANE", 0, 0, 0,
True, 0, Nothing)
Set SWFeature = MySWAssembly.AddMate2(0, 0, False, 0, 0, 0, 0, 0,
0, 0, 0, longstatus)

As for the Lookup Table statement, I think I should have used a
different term. Yes Excel has a native lookup function that would work
just fine, but I would recommend *not* involving Excel in this mix
unless you have to because you're just adding more complexity (that I
think you don't need to get into for this project). For now (or maybe
at least for starters), just keep all the code and conditional stuff
inside your macro. The lookup I was talking about was something along
the lines of:

Sub main ()
Set swApp = CreateObject("SldWorks.Application")
Set MySWAssembly = swApp.ActiveDoc

<<<All your code to read in the dimension value, I'll call it DimVal>>>

'Poor man's Lookup Table to get Filename of Component to Insert into
Assembly
Dim MyInsertComponentFilename as String
If DimVal = 0.250 Then
MyInsertComponentFilename = "0.250-SHAFT.SLDPRT"
ElseIf DimVal = 0.500 Then
MyInsertComponentFilename = "0.500-SHAFT.SLDPRT"
ElseIf DimVal = 0.750 Then
MyInsertComponentFilename = "0.750-SHAFT.SLDPRT"
ElseIf DimVal = 1.000 Then
MyInsertComponentFilename = "1.000-SHAFT.SLDPRT"
Else
MsgBox "Error. Filename for " & DimVal & " Not Found."
End
End If

<<< Stuff to Insert and Mate your Component, or whatever you you want
to do. >>>>

End Sub
 
This code can also be written with the "Select" command in vb - does
exactly the same thing, but sometimes makes more sense (to me anyways)

rewritten...

Dim MyInsertComponentFilename as String

Select Case DimVal

Case 0.250
MyInsertComponentFilename = "0.250-SHAFT.SLDPRT"
Case 0.500
MyInsertComponentFilename = "0.500-SHAFT.SLDPRT"
Case 0.750
MyInsertComponentFilename = "0.750-SHAFT.SLDPRT"
Case 1.000
MyInsertComponentFilename = "1.000-SHAFT.SLDPRT"
Case Else
MsgBox "Error. Filename for " & DimVal & " Not Found."
End Select
 
Thanks for all of your help guys... I will see what happens when I
implement this... Thanks again...

Jeff
 
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