NX8.5 Cylindrical Dimension drafting glitch 1

[braddles90]

Hi all,

Just wondering whether anyone else has seen this glitch? When I'm in drafting mode, say I have a rectangular plate with an 8 hole pattern through it, and I put a section through the plate to show the holes through the thickness of the plate. I put two 2D centrelines through the holes in the section, then when I go to put a Cylindrical dimension between the centrelines to show the PCD, the dimension doubles the actual value (i.e. if the PCD is modelled at 100mm dia., the dimension will show up as dia. 200).

Hopefully my example is clear enough (I can post a sketch if needed) - anyone able to say they've seen it before, or why it does it? It's a pretty annoying (and potentially dangerous, because I've only just caught it a couple of times after checking the drawing)!

Thanks!

 

[Toost]

This is as designed. If you select the centerline as first object NX will double the value. If you select the outline as first it will not.

The reason is if you have a section view where only one of the outlines is visible, you can still place the full diameter using the centerline as the second object.
( Then turn off the arrow to the centerline.)

Regards,
Tomas

 

[Toost]

and a picture.

Regards,
Tomas

 

[ewh]

I find this a handy feature rather than a glitch. There are work-arounds for what you are trying to accomplish - dimension to the actual edge centers instead of the centerlines, dimension your BC in the view from which your section was derived, or use vertical or horizontal dimensions with the diameter symbol appended.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[braddles90]

Cheers guys, sorry for the late reply.

Seems a bit strange to build that kind of combined function into the one command, where it changes the shown dimension depending on where you select - seems fraught with danger to me (but once you understand what its for it's pretty handy I guess).

The workarounds are a bit annoying, hence why I asked the question - using normal linear dimensions and appending the diameter symbol doesn't look right when making the dimension basic or reference (the brackets or box don't encapsulate the added text), and selecting the geometry as the dimensioned point then overlaps the dimension and the centreline so you have to go play around with the end spacing. Not major gripes, just a few little annoying things!

Thanks again for the clarification.

 

[Xwheelguy]

So put a Circular Centerline through the PCD in the top view instead of the section and use the Cylindrical Dim. there with basic dim. callout.

As others have said, it's working as designed and has worked that way ever since I can remember (UG v11?). If you're able, add a centerline for the PCD in the section view and dimension from there and it will double the radial value (but show a Ø symbol correctly, even when basic).

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB