API Object - Extrude:getfaces

This is my first attempt at using the API and I am stuck on a particular
problem.

I am creating a dome feature on an existing extrude feature, and believe I
know how to handle the feature however I am having trouble getting it. The
feature in question is named so I ideally would like to get the feature by
name then perform a getfaces on it.

Just to clarify, I can select it into the SelectionMgr but I believe I need
define the object in order to perform a getfaces.

Hope this makes some sense.

Thanks
-hack

 

Could you post the code used to create the extrude feature.
When working with objects that you created in the same macro it isn't
advised to select them by name. IMHO Anyway if you post the code I could
show you how to get the feature object

Corey

 

Part.ClearSelection2 True
boolstatus = Part.Extension.SelectByID("CircleSketch" & strCutNum, "SKETCH",
0, 0, 0, False, 0, Nothing)
Part.FeatureManager.FeatureCut False, False, False, 0, 0, Lc, EightInch,
False, False, False, False, 0, 0, False, False, False, False, 0, 1, 1
Set ThisFeatureCut = Part.FeatureByPositionReverse(0)
ThisFeatureCut.Name = "Cylinder_" & strCutNum
Part.ClearSelection2 True

You can see that I access a sketch created within the macro called
CircleSketch** on which to build my extrude. I could do the same thing for
the extrude feature, however I need to perform some face tests (as you
probably recall) so a simply selection isn't sufficient (I believe).
Please note that I use no absolute coordinates anywhere in the macro, as
they are ultimately provided by a user data file.

Thanks
-hack

 

Try this

Dim ThisFeatureCut as Feature
Dim ThisFeatureSurfaces as variant

Part.ClearSelection2 True
boolstatus = Part.Extension.SelectByID("CircleSketch" & strCutNum, "SKETCH",
0, 0, 0, False, 0, Nothing)
set ThisFeatureCut = Part.FeatureManager.FeatureCut (False, False, False, 0,
0, Lc, EightInch,
False, False, False, False, 0, 0, False, False, False, False, 0, 1, 1)

If thisfeaturecut is nothing then
msgbox "Feature Cut Failed! Aborting Operations."
end sub
end if

'you shouldn't need the next line now
'Set ThisFeatureCut = Part.FeatureByPositionReverse(0)
ThisFeatureCut.Name = "Cylinder_" & strCutNum


ThisFeatureSurfaces = thisfeaturecut.GetFaces

msgbox "Found " & str(ubound(ThisFeatureSurfaces) + 1) & " faces on feature
" & ThisFeatureCut.Name

Part.ClearSelection2 True

Regards,
Corey

 

Thanks again CS.

Is there any easy way to get a look at the contents of the array now.

I have the array ThisFeatureSurfaces now containing 2 elements as per your
msgbox.

I tried to just do a simple:

For each i in ThisFeatureSurfaces
MsgBox "This face info: " & ThisFeatureSurfaces(i)
Next

just to get a better handle on the contents here. This fails with object
doesn't support this property or method. If I enclose ThisFeatureSurfaces
in a Str() function I get a data mismatch.

I will then test the surfaces to understand which is the flat surface so I
can continue to use it for the next feature.

 

Well you can add a watch by selecting the variable and RMB>Add Watch the
only thing this will give you is a list showing that you have two valid
objects and possibly that they are of Face2 type. If you want to see the
surfaces that are selected you could do this.

Dim ThisSurfaceEnt as Entity

for each i in ThisFeatureSurfaces
Set ThisSurfaceEnt = i
ThisSurfaceEnt.Select4 false, nothing
msgbox "Do you see the surface that is selected?"
Norm = i.normal
Face2.
if Norm(0) = 0 and Norm(1) = 0 and Norm(2) = 0 then
'this is a cylindrical surface don't do anything
msgbox "The selected Face is probably cylindrical"
else
'Norm is the direction vector. Compare this to a known
msgbox "The selected Face is probably Planar"
If 'some vector comparison then
set WantedFace = i
end if
end if
next

 

Woops the line that says "Face2." needs to be deleted.

Corey

 

I'm curious how is this working or not.

Corey

 

Thanks for your interest. What I have done is created and circular extruded
cut into a rectangular solid such that a third of the circle is outside the
block. the Extrusion only penetrates the block to about 1/3 depth. From
here my goal was to add an extrusion to the back of the extruded cut, such
that I would now have a backing if you will of the same shape, which travels
an additional 1/3 into the block. Once this was complete I would then add a
dome feature to my extruded "backing" to blend it into the block.

I have completed all of this from 2 points pulled from a data file,
however I have been unsuccessful creating the dome. I have used the getfaces
method to obtain the faces of the backing and I think ruled out the
cylindrical face, however, cannot figure out how to eliminate the front face
of the extrusion and then how to select the remaining face to use as the
origin of the dome.

I have tried posting screen caps to explain this better, but when I did the
posts would not show up.
I could probably post these pics on a website for you to view if that would
help.

Thanks
hack

 

If you e-mail me your code and example files to run I could maybe get it
working for you.
Pictures might help. But would leave me with no real way of expiramenting.

Corey

 

Oops I for got



Remove eroneous info.

Corey

 

For future reference this works

Dim NormalVofCut as MathVector
Dim NormalVofThis as MathVector
'.........

ThisFeatureSurfaces = ThisFeatureBackStop.GetFaces

Debug.Print "Found " & Str(UBound(ThisFeatureSurfaces) + 1) & " faces on
feature" & ThisFeatureCut.Name

For Each i In ThisFeatureSurfaces
Norm = i.Normal
If Norm(0) = 0 And Norm(1) = 0 And Norm(2) = 0 Then
Debug.Print "This face is cylindrical"
Else
Set WantedFace = i
Set NormalVofThis = GetNormalVector(WantedFace.Normal)
Debug.Print "Normalised:" & NormalVofThis.GetLength
'Corey: check to be sure the vector of this surface doesn't
match the
'bottom of the origional cut. They should be exact opposites.
If Not NormalVofThis.ArrayData(0) = NormalVofCut.ArrayData(0) Or
_
Not NormalVofThis.ArrayData(1) = NormalVofCut.ArrayData(1) Or _
Not NormalVofThis.ArrayData(2) = NormalVofCut.ArrayData(2) Then
'select the surface
WantedFace.Select4 True, Nothing
'MsgBox "This should be your face"
Exit For
End If
End If
Next
'Corey: set the mark as required by the dome feature
SelMan.SetSelectedObjectMark 1, 1, swSelectionMarkSet
Part.InsertDome 0.007, False, True
'.........


Function GetNormalVector(Normal As Variant) As MathVector
'Corey: make sure the vector is normalised
Dim MathUtil As SldWorks.MathUtility
Dim NormalPoint As New MathPoint

Set MathUtil = swApp.GetMathUtility
Set NormalPoint = MathUtil.CreatePoint(Normal)
'NormalPoint.ArrayData = Normal

Set GetNormalVector = NormalPoint.ConvertToVector
Debug.Print GetNormalVector.GetLength
Set GetNormalVector = GetNormalVector.Normalise

End Function


Regards,
Corey