I use the "Ground and root component" button quite often, but now that we went to 2012 64bit, some (most) parts i try will not ground and root, while some will. Any ideas?
Thanks
Chris
I know that i cannot help you but only for your information in my system which is similar to your the "Ground and root component" works very well.
1. Make sure the part is not already grounded. I know that sounds simply, but I have done this.
2. Make sure you are in the Master positional rep. You should get a message saying "Unable to ground and root component" if you are not in the master PR.
Other than that, it "should" work.
#2 is a good one to remember i didn't know that! Could easily see getting caught out with that. I wish Autodesk would change the ground n root command, its awful! Its technically very bad fully constraining all the parts & then grounding them as well. Its effectively over constraining them! Its also more stuff for inventor to calculate when opening the assembly. Its should reset the parts origins to 0,0,0 and then ground the part. I know thats how Kent Kellers Insert n Fix add-in worked. But so should Autodeks, its the simplest and best way to do it. We have written a macro to use instead!
Scott Moyse
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Design & Manufacturing Technical Services Manager at Cadpro New Zealand
Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project
One other thing...you cant be in the context of an assembly. You will have to open the subassy explilcitly before the command will work.
I kno.... it sux, but that is just the way it is.
Yep, thats what it is. It seems as if you have the assembly open that you are trying to ground and root the part in by it self. I always open the main assembly. I have two parts to insert, one in each sub assembly. I open the main assembly , double click the first sub assmebly, then insert my part, ground and root, then double click the other sub assembly, insert the part, ground and root...
Why did they change this? Is this a bug?
At least I know what is causing it now. thanks
Thats the new and improved version ...
It worked in 2010, but then they broke it in 2011. If I remember right, this tool wasnt officially supported until 2011. Prior to 2011, these bonus tools were used as-is. In 2011 they included these tools with the installation. That is when they became broken. The bug in 2012 is just a copy of the bug in 2011.
@karthur1 wrote:Thats the new and improved version ...
It worked in 2010, but then they broke it in 2011. If I remember right, this tool wasnt officially supported until 2011. Prior to 2011, these bonus tools were used as-is. In 2011 they included these tools with the installation. That is when they became broken. The bug in 2012 is just a copy of the bug in 2011.
just to clarify, these commands were included in 2010 out of the box, previous to 2010 they were bonus tools.
in either case this in yet another example of Autodesk breaking things that worked and allowing them to stay broken release after release, or introducing commands that are left not fully working release after release. it seems to be getting worse and worse.
I've asked a guy I know if he is willing to share a simple bit of VBA code he has to replace the need for this command. He gave it to us, but it's not my place to give it out. He's a good fella, so i'm sure he will come to your aid.
Not sure why we should be creating code to fix up Autodesk's crappy work. But i will add the SP1 beta is not far away, if you have issues like this get in early and report them, you never know they might be fixed by sep/oct.
Scott Moyse
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Design & Manufacturing Technical Services Manager at Cadpro New Zealand
Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project
He is cool with it, Cheers Brian Corbin! Here you go guys use this:
Public Sub GroundParts()
Dim oDoc As AssemblyDocument
Set oDoc = ThisApplication.ActiveDocument
If oDoc.SelectSet.Count = 0 Then
MsgBox "Select some parts first", vbExclamation
End
End If
Dim oSelectedOccs As ObjectCollection
Set oSelectedOccs = ThisApplication.TransientObjects.CreateObjectCollection
Dim I As Long
For I = 1 To oDoc.SelectSet.Count
If oDoc.SelectSet.Item(I).Type = kComponentOccurrenceObject Then
oSelectedOccs.Add oDoc.SelectSet.Item(I)
End If
Next
Dim oOcc As ComponentOccurrence
For Each oOcc In oSelectedOccs
If oOcc.Constraints.Count <> 0 Then
MsgBox oOcc.Name & " has constraints on it and will be skipped"
GoTo skip
End If
Dim oTransform As Matrix
Set oTransform = oOcc.Transformation
oTransform.SetTranslation ThisApplication.TransientGeometry.CreateVector(0, 0, 0)
Call oOcc.SetTransformWithoutConstraints(oTransform)
oOcc.Grounded = True
skip:
Next
End Sub
There is one thing to bear in mind when using this code. If the part is rotated in any way between placing the part and using your button, then it won’t zero out the angular occurrence. You can probably modify the code so it resets the angular occurence as well, but we haven't got round to it yet, and is easy enough to work around as long as you know it can be a problem. It's generally fairly obvious when it happens.
Scott Moyse
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Design & Manufacturing Technical Services Manager at Cadpro New Zealand
Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project