Hole wizard in end of solid of revolution...

[MikeHalloran]

2009.4.1

I thought thread559-164556 had the answer to my problem.

I try and try and try pre-selecting, and I can't make the Hole Wizard produce a 2D sketch.

I'm trying to put a 2" pipe port in the end of a revolved cylinder that's 2.6" diameter on the end face.

The wizard will let me put it anywhere _except_ dead nuts on center. If I preselect using the filter 'planes' only, SW leaves a tiny bright cross on the selected surface, and puts the damn hole right there. If I try to post-select while looking straight at the surface, just as I get to the center, when the target becomes an open circle with a cross in it, just as I select, the target changes to a black dot.


I get either "Sketch points cannot be created at the same
location as an existing point", which refers to the point at the intersection of the centerline and the radial line that produced the solid of revolution in the first place, which is _exactly_ where I want the center to be,

or I get "The hole could not be located due to geometry conditions."

or I get the accursed "Points to locate holes are not valid. They may not be constrained or may be located on edges or vertices." That second sentence makes no sense whatsoever to me.


Here's a simple test that reproduces the behavior.
On the Right Plane, sketch a corner rectangle 1.3" high and 6" long.
Revolve it around the longer edge through the Origin.
( No, I wouldn't make a simple cylinder that way, but the part that's giving me trouble is not simple. )

Now use the Hole Wizard to put 2" pipe holes in the ends.
You CAN put a hole dead center in the end that doesn't intersect the Origin.
You CANNOT put a hole dead center in the end that intersects the Origin.
Okay, maybe you can; I can't.

Well, once, I got it to make a hole by drawing centerlines on the Origin face, but I couldn't do it twice in a row.

Any ideas?




Mike Halloran
Pembroke Pines, FL, USA

 

[CorBlimeyLimey]

This is one of the works of SolidQuirks quirks of SolidWorks. A HW point cannot be created on top of an existing point ... but a created point can be dragged onto an existing point.

Makes perfect sense, right?

 

[CorBlimeyLimey]

The HW is being changed with SW2010, but I don't believe it addresses your, umm, point.

http://www.mikescadblog.com/2009/08/whats-new-in-solidworks-2010-hole-wizard-2d-sketch.html

 

[NomLaser]

CBL has the solution. Select the surface that you want it placed on then start the HW. You can create a point anywhere but where you really want it. So you put the point in space and drag it onto the center or over an existing point.

 

[MikeHalloran]

Okay, I'll try dragging the point tomorrow.

I'm sure it all makes perfect sense on SW's home planet.





Mike Halloran
Pembroke Pines, FL, USA

 

[MikeHalloran]

Yep, works.
Yecchh.

Thanks.


Mike Halloran
Pembroke Pines, FL, USA