I updated a Pipe Support Part file . But.. when I opened the drawing file, I saw the views missing (along with dim & annotation).
Do a rebuild of the model, save it again and then see if the views have updated on the drawing.
Tried rebuild, but did not work. However, one thing I noticed. Right clicking on the missing views gives the option to open that part file. but, the View remains empty.
A few versions back I had it happen ever so often with a view and the trick then was to delete the offending 'empty' view and then undo the delete.
That somehow made SW wake up and recalculate and redraw the view.
The other visible view on right side; are they of the same part. If not then did you changed the part Or moved it to a different location then please make sure references in the drawing are correct OR they're looking int the right path.
other visible views are of the same part file. Basically, I am trying to save individual Pipe Support into different part using "Insert into New Part.." command and show all of them in one drawing, separately.
Saeenath Sutar wrote: I am trying to save individual Pipe Support into different part using "Insert into New Part.." command and show all of them in one drawing, separately.
Saeenath Sutar wrote:
I am trying to save individual Pipe Support into different part using "Insert into New Part.." command and show all of them in one drawing, separately.
If you're only doing this to detail bodies for a drawing are you aware of the "Select Bodies..." button? That makes it very easy to create drawing views of single bodies without the need to save bodies out as separate parts.
What is your specific need that you want all of them as separate file. If just want them to detail in same drawing then use the Glenn's method.
In case there is a different issue then please upload complete files here to check.
Views hiding at random has been an ongoing issue in my work. Toggle hide/show view will bring it back or a rebuild. Show/hide is faster. SW is somewhat lacking speed & reliability in drawings. Below is a code that I have modified (Kudos to the original owner!), it toggles hide/show the selected view or if no view selected goes through all views and toggles them on/off. That little code has saved me many clicks and time...
Dim swApp As SldWorks.SldWorksDim swModel As SldWorks.ModelDoc2Dim swSelMgr As SldWorks.SelectionMgrDim swView As SldWorks.ViewDim vViews As VariantDim vView As VariantDim myView As SldWorks.ViewSub main() Set swApp = Application.SldWorks Set swModel = swApp.ActiveDoc Set swSelMgr = swModel.SelectionManager On Error Resume Next Set swView = swSelMgr.GetSelectedObject6(1, -1)
If Not swView Is Nothing Then 'MsgBox "You have selected " & swView.Name swView.SetVisible False, False swView.SetVisible True, False Else 'MsgBox "no view selected " vViews = swModel.GetCurrentSheet.GetViews1000:For Each vView In vViews Set myView = vView If Not (Left(myView.GetName2, 1) = "*") Then myView.SetVisible False, False 'swDwg.EditRebuild3 myView.SetVisible True, False End IfNext vView End If
swView = NothingmyView = NothingswApp = NothingswModel.ClearSelection2 (True)Set swView = swSelMgr.GetSelectedObject6(1, -1)End Sub
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