Hello
I do it via the visualization cube.
OBI WAN and ac cobra 427, all this works well for all bodies except the Sheet...
With the visualization cube, the dimensions of the folded and not unfolded part are obtained .
Good... the method I'm going to use in the meantime is to copy this expression in the "Description" field :
Sheet Thickness "SW-Thickness of tôlerie@@@SW-CutListItemName@SW-FileName(FileName)"... "SW-Flank Length tôle@@@SW-CutListItemName@SW-FileName(FileName)"x"SW-Flank Width tôle@@@SW-CutListItemName@SW-FileName(FileName)"
The ideal would be to be able to copy it in the field normally occupied by "Sheet" (see pj), but as max59 said, no way to copy a special character there ...
2019-02-27_14h33_20.png
1 Like
I maintain the idea of the Macro,
Personally I have a macro for the recording that does:
- Dimetric view
- Zoom at your best
-Check in
=> all connected to an "S" key which means that by pressing S the model rotates, zooms in at best and saves.
=> It is possible to integrate the macro that injects the variables into a routine macro like this one, it will reinject the variables at each record but at least they will be there!
I use this system and having gotten into the habit of recording only via the macro, it's much more flexible, you can do what you want with it, it works for new and old parts.
I added in my macro a deletion of variables, an addition of new ones and it works great!
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I'm not very familiar with macros, but I do have the impression that I'll have to go through it.
Michael, I'll test your code when I have some time.
I will keep you posted.
Hello, maybe another lead.watch at 23min 23 s
https://www.youtube.com/watch?v=Pjqi1XSLY5A
may the force be with you.
Michael DELACOTE, could we add to your macro the fact that it only applies the designation to bodies called Tole and not to profiles:
And if so, what is the piece of code to modify/add?
Thanks in advance!
Hello
Here is the modified code, the Cutlist article must start with "Tole" otherwise it won't work.
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swFeat As SldWorks.Feature
Dim swCustPropMgr As SldWorks.CustomPropertyManager
Dim NF As String
Dim Liste As String
Dim Final As String
Dim st As String
Dim swBodyFolder As SldWorks.BodyFolder
Dim swBody As Body2
Dim vBody As Variant
Dim i As Integer
Sub main()
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swCustPropMgr = swModel.Extension.CustomPropertyManager("")
NF = swModel.GetTitle() & ".SLDPRT"
st = """"
Set swFeat = swModel.FirstFeature
Do While Not swFeat Is Nothing
If swFeat.GetTypeName() = "CutListFolder" Then
Liste = swFeat.Name
Set swBodyFolder = swFeat.GetSpecificFeature2
swBodyFolder.UpdateCutList
Final = st & "SW-Longueur du flanc de tôle@@@" & Liste & "@" & NF & st & "x" & st & "SW-Largeur du flanc de tôle@@@" & Liste & "@" & NF & st
If Liste Like "Tole*" Then
Set swCustPropMgr = swFeat.CustomPropertyManager
swCustPropMgr.Add3 "Dimension", swCustomInfoText, Final, 1
End If
End If
Set swFeat = swFeat.GetNextFeature
Loop
End Sub
3 Likes
Excellent! It works ;-)
Thank you Michael
2 Likes
Thank you Michael for your macro!
Hello
I'm new to the group. Here is the solution I use.
by creating a custom property form for sheet metal.
PL. "SW-Thickness of tôlerie@@@PLAQUE@Pièce1.SLDPRT" X "SW-Width of tôle@@@PLAQUE@Pièce1.SLDPRT" X "SW-Length of tôle@@@PLAQUE@Pièce1.SLDPRT"
I like the idea of the macro to Michael DELACOTE.
Have a nice day!
propriete_piece_de_tolerie.pptx