on 06-07-2017 07:02 AM
I have been asked by a colleague if it is possible to apply a cylindical dimension to a revolved body using PMI, the catch is, it needs to be displayed in a particular orientation.
I have attached some images of what we want to achieve and what NX is giving us...
Any help on this will be greatly appreciated.
06-07-2017 07:51 AM - edited 06-07-2017 08:03 AM
Hi, unfortunately I only know a workaround (I'm working on NX10):
- create a datum plane trough the center of the cylinder
- crete intersection curves cylinder and datum plane
- make a dimension between the intersection line
- to an relation for the dimension to the cylnder face you can add
the cylinder face to the dimension using "assisiated objects"
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on 06-07-2017 08:23 AM
The easiest way would be creating the section view (through the center of your cylindrical feature) from one of your Model Views.
Then, follow the steps below:
I hope it helps,
on 06-07-2017 08:31 AM
Create a PMI rapid dimension.
Go to Orientation and plane. Select user defined plane and select a plane that goes through the center of the shaft and what plane you want your dimension to sit on.
Then select a point at the top of the diameter edge, and select the bottom point of the same edge. This should get you the dimension you have shown. then select the face to associate your PMI dimension to. Hopefully this may work for you.
06-07-2017 08:31 AM - edited 06-07-2017 09:15 AM
06-07-2017 09:12 AM - edited 06-07-2017 10:13 AM
Another way as @Lezajsk21294 mentioned, create the cylindrical dimension in section view then it can be displayed in the other views as needed. But it needs to keep the section view otherwise if section view is deleted then the PMI shown in other views will loose their associativity.
Just note that in NX 10 there are options 'Create Section' and 'Create Lightweight Section View'. From NX 11 there is only option 'Create Sectio View'.
on 06-07-2017 11:05 AM
Thanks for all the replies,
We have managed to work through the different methods shown, but feel that we should be able to just select the face (PMI Best Practice), specify that a cylindrical dimension is required and which orientation it should be on.
Having to set the plane, then pick tangent points, then select the associated faces is the work around, right up untill there is a chamfer or radius on the reference edge that changes...
Maybe an Enhancement Request for @dwingrave?
on 06-07-2017 05:11 PM
Mike, I'm trying to understand your concept from your description. How would you specify "which orientation" the PMI should be placed if not for determining/specifying the Annotation Plane? Just curious.
However, I have another viewpoint on this whole subject. What's the purpose of placing that diametral dimension in the first place? Doesn't the geometry topology of the Solid provide that information? Why do you want to have PMI respecify what the Geometry already specifies? Why do you need it as you've indicated your desired orientation?
I'm not saying NX's PMI display/placement options don't need to be enhanced... (For instance, I would like to be able to just have a single leader attached to the Face Edge (Which isn't an Arc, because the End Face isn't perpendicular to the Cylinder Axis, for instance.) and have it reflect the Cylindrical Diameter of the Face with the Diameter Tolerance, in order to attach a corresponding FCF with a Postion or Profile Tolerance to enable specifying what Bonus Tolerance at MMC for instance..., where I could have the Annotation Plane be either perpendicular or parallel with the Cylindrical Axis.)
on 06-08-2017 02:56 AM
Apologies for the confusion, It sounds like we want exactly the same enhancement, Ive just used the wrong terms.
The reason we need to put diameter dimensions on solid views, rather than a section is to produce a drawing (Our customer still has a requirement for this). Maybe we need to review how we produce detail drawings, we are still experimenting with PMI at the moment, that said, with difficult proceedures comes resistance to use the software.
The problem is as you describe, when you select the cylindrical face, NX wont allow it to be placed on a plane in line with the cylindrical axis, it only goes in the same plane as the end face.
I'll have a look and the GTAC ER page and see if there is already a request along similar lines, then either add to it or create a new one.
Thanks again for all the help.
on 06-08-2017 04:24 AM
I have attached the movie, where you can see, that those dimensions can be placed with PMI Linear Dimension. You just have to add diameter symbol. And before placing the PMI, make work the view, in which you want to place dimension.
Is this, what you were looking for?