API Feature Selection

I am trying to create a simple dome feature on a cylinder face that is also
created from within my macro. The problem I'm having is that I do not know
how to select the appropriate face on the cylinder by name.

The line:

boolstatus = Part.Extension.SelectByID("", "FACE",
0.02256158044904, -4.995574477107E-04, 0.004999999999995, False, 1, Nothing)

was created by the macro record function when selecting the face using the
GUI. There is no way I can use absolute coordinate values so I want to be
able to use the name parameter (first set of "").

The cylindar has three surfaces so can someone please tell me how to name
the correct surface on the cylindar during creation such that i can use it
in the creation of my dome

thanks a bunch
-hack

 

You can access the surfaces through the Extrude features faces

Then you will have to check to see if the surface is cylindrical If it is
discard it. Now you are left with your other 2 surfaces. You will have to
compare them by their normal direction.

Feature::GetFaces
Dim Faces as variant
Dim i as variant
Dim Norm as variant
Dim WantedFace as Face2

Faces = MyFeature.GetFaces
for each i in Faces
Norm = i.normal
if Norm(0) = 0 and Norm(1) = 0 and Norm(2) = 0 then
'this is a cylindrical surface don't do anything
else
'Norm is the direction vector. Compare this to a known
vector
If 'some vector comparison then
set WantedFace = i
end if
end if
next

WantedFace.select4(false, nothing)


Regards,

Corey

 

I am a little unclear on some of your code:
I assume the getfaces method will put the three faces of the cylinder
into the array faces.
(I'm not clear on what is actually stored in the array and how that refers
to the face)
Then you are going to test each face's normal vector??

I'm not sure what the test statement does in order to id this face as the
being cylindrical:
if Norm(0) = 0 and Norm(1) = 0 and Norm(2) = 0 then
What does a value of 0 constitute.

Then, if i am able to narrow the selections down to the 2 opposite surfaces,
how can I differentiate between them. I would assume they both share the
same normal vector albeit offset. Note I will be using a point (that is
named) and subsequent plane, to initiate the sketch for the first side of
the cylinder. Perhaps some characteristic of this point or plane can be
compared to something on the "not wanted" surface to identify it and
subsequently reject it.

sorry if some of my questions seem crazy, I am very new to the API.

-hack

 

see comments below

Regards

Corey

It is a pointer to the face object this can be passed to a variant or object
or Face2 variable.

The normal vector is a point and a direction can be figured in relation to
the origin. If the face is not planar Face2::Normal returns an array
[0,0,0] so in the if statement you are able to check if the face is planar
or not

Actually they shouldn't they should be exact opposites because the normal
vector would be the direction away from the solid body the OUT direction if
you will.

I would maybe compare the normal direction of the sketch to each face. I
presume you want the end away from the sketch. If you extrude it without
flipping the extrution the normal of the sketch and the normal of your face
should be the same direction. The next problem is going to be that even
though 2 planes may have the same normal direction you may have a point
further out on the direction vector for one than the other. You may want to
compare ratios instead of a direct comparison.

x1/y1 = x2/y2 and z1/x1 = z2/x2

but then you have to watch out for divide by zero.

Maybe someone else has had to compare Direction Vectors in SW and could
enlighten us on how they handled the comparison.

Corey

Questions are never crazy it is just that sometimes you don't know anyone
with the right answer.