The program won't let me loft between profiles in a workplane set

[vgillespie]

Hi folks,

I am using Creo Elements / Direct Modeling Express.  I am trying to loft through three profiles on three workplanes in a workplane set.  The profiles are fairly simple shapes with four vertices each.  But one of the workplanes is perpendicular to another one and one edge of the profile on one is coextensive with one edge of a profile in another workplane (and I think that may be causing a problem).  Anyway, when I try to create an appropriate matchline I get an error message which says: "If a vertex lies in another workplane, a vertex must be at the same position in the other workplane."  I don't know what that means and cannot create a loft between the three profiles on the three workplanes.  What must I do to create this loft?  I have attached a drawing with the three workplanes so you can see what I am talking about.

Thanks in advance,

Vincent

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[mchristensen · Accepted solution]

Vincent,

Had the same problems with three orthogonal planes (x-y-z) and a curve in each.  The geometry of the planes must be inspected VERY closely to make sure that they really do intersect.  I found that the 3D Geometry/ insert face command worked better than the matchline (with plane sets) and loft method.  Even with insert face, the points have to micro-intersecting - took me several tries to get it right when creating the curves.

my geometry is attached.

Mick Christensen

USS Midway Museum

[vgillespie]

Hi Mick,

After I posted my question I saw that in the help file it said that when you are lofting with a workplane set "[i]f two workplanes share a common edge, then any additional workplanes must also share this edge."  (If you want to read about that go to the help file and get the help page titled "Lofted Freeform Parts," then scroll down to the section titled "Lofting Around A Common Edge.")  Then I understood what was happening.  When I understood that I was finally able to make the part I was making by doing it in two separate pieces.  First I created the portion of the part with the two profiles that shared an edge and then I created the rest of the part by using the remaining profiles (which did not share that edge) and having them loft to the portion of the part I had already created.  (Only one profile was needed for the second portion of this operation.  But it seemed that the program did not like me using only one profile to loft to a part.  Thus, I added an extra profile [on a new workplane] for this operation and then later cut off the excess portion of the resulting part.) 

Then I got your reply.  I did not know about the "insert face" command.  I went ahead and recreated the part using that command earlier today.  I then used the "gather faces" command to change the set of faces into a regular part.  It worked just fine (after I spent a little time with it and learned how to use these commands).  It is good to know about this.  I will probably be using these commands in the future.

Thanks for your reply.

Best regards,

Vincent