custom reorienting detail view normal to plate in DRAFTING???

[vasinka]

I am making a drawing of a rectangular frame (out of steel sq tubes) the top of frame has small 5"x5" plates welded on top of every vertical post.
There is no symmetry to this frame, its like a snake where the top two longerons are cut at a unique angle at every vertical post.

Problem:
I must give detail view of every plate.
If I grab detail view from the top view that I have of the frame, detail view is NOT normal to the plate.

question:
Is there a way to re-orient my detail view normal to the plate without parent view being normal at that location?

Things I tried.
1. after I right click and make that detail independent, I have "orientation" option in the Settings>Detail>settings>Orientation.
This allows to pick normal and x-vector and attempts to orient the view, but i get an error of "can't place view outside of deg boarder"
I made sure that "anchor point" of detail view is in center but that doesn't fix the issue.
2. I can create break out view, or create view and use custom border to only show desired view. -that's too much work!

Using NX10

 

[NutAce]

As a Workaround, try and make your sheet as large as possible. Edit the views and change the sheet size back again.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX11 / TC11

 

[Xwheelguy]

Alternatively, you could create Custom Views in Modeling with the plates oriented as needed and just drop those saved views onto your drawing and not worry about specifically calling them out as details - label them as true top view or something to that effect. Another option is to place Datum CSYS at specific locations such that the axes will allow you to use the orient button while placing a model view - saves the time from doing the save view steps - can make the orientation associative to the Datum CSYS and if your part moves around, you should be able to relocate the Datum CSYS & drawing views should update accordingly.

Tim Flater
NX Designer
NX 11.0.1.11 MP4
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[SDETERS]

You could also make a section view that is aligned with a plane, and call it a view.

 

[alphawell]

Hi, vasinka. It's not quite clear for me what is your model look like, but I suppose this can help you.
What you really need is to orient drafting view while creating it. Try to create new drafting view via Base View command or View Creation Wizard (that really does not matter). I'll explain with Base View command, as I usually use it for these purposes. In the options dialog box, in the Model View group, there is an Orient View Tool button. Pushing it will open corresponding command options dialog and orient view window. All you should do here is specify two vectors: for normal direction, and for X (horizontal) direction. It's possible to use any objects of your master-model and various methods of vector definition to specify these directions. For example, you can assign Normal Direction of view to match the normal of one of your "5x5" plate's face, and horizontal direction to either of its edges. This is really quick and advantageous approach, try it.

 

[DonNX]

A method that I've used before is the following:

1. While in DRAFTING go to the MODEL (Ctrl+M).
2. Change your selection filter to FACE.
3. Orient the view with you mouse to close to the orientation you want & press F8 (The view will now be perpendicular to the selected face).
4. Now go Menu>View>Operation>Save_As & give each view you create a unique name by typing it in the Name box & clicking OK.
5. Go back to Drafting (Ctrl+Shift+D).
6. Use the View Creation Wizard to place a new view (Ensure that you're using the specification of the part under loaded parts & not the part as such).
7. When you reach the Orientation tab you should see the views you created under the Model Views window, select the view you want to place & place it in your drawing.

Hope this helps,
Don

"It is impossible to make anything foolproof because fools are so ingenious."