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Half cylindrical view in drafting NX 9

Valued Contributor
Valued Contributor

Hi,

 

Can anyone tell me how to create half cylinder view in NX 9 drafting.

For eg. Consider a cylinder of dia as 50 and Length as 200, if I would like to show the upper portion of the cylinder from the center line how can I show. I don't want to show bottom portion of the cylinder as it is symmetry.

 

Please help if someone knows.

 

Thanks,

Yunus

7 REPLIES

Re: Half cylindrical view in drafting NX 9

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Have you tried "view break"?

Re: Half cylindrical view in drafting NX 9

Siemens Phenom Siemens Phenom
Siemens Phenom

You could also consider just redefining the boundary of your view so that only half of your cylinder is visible in the view. Just right-click the view boundary, select Boundary, change the boundary type to Manual Rectangle, and then drag a rectangle around the portion of the view you want to be visible.

 

Here are some Help topics that might also help you add dimensions to a view like this:

 
 

Re: Half cylindrical view in drafting NX 9

Valued Contributor
Valued Contributor

Hi,

 

Thanks for your reply. There is some issue with View Break in NX 9. If we use view break you can't see center line of the component. It will get hide automatically by giving information dialogue.

 

Thanks,

Yunus

Re: Half cylindrical view in drafting NX 9

Valued Contributor
Valued Contributor

Hi,

 

Thanks for your reply.

 

If we use View Boundary as Manual Rectangle there are some of the visible lines below the center line of the component till the View Boundary. I don't require any of the visible lines below the center line of the component. I want to see the component view exactly above from center line of the component. Let me know if you have an alternate solution for this. It will be great help if solution exists.

 

Thanks in advance.

Yunus

Re: Half cylindrical view in drafting NX 9

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Well, it's a labor intensive solution, but there is always "view dependent edit".

Re: Half cylindrical view in drafting NX 9

Siemens Phenom Siemens Phenom
Siemens Phenom

Well, if you use the view break method, here is a procedure that will let you "name" the centerline, and then use that name as a selection object in the Linear Dimension dialog box. That way you can hide the centerline (because it is outside the bounds of the view) but still use it to create dimensions.

 

Create a named centerline, and then hide it:

  1. Create your view, and then add a view break.
  2. Choose Home tab→Annotation group→3D Centerline and add a centerline to the view. Note that it may appear outside of the drawing border.
  3. Right-click the centerline symbol and select Properties.
  4. On the General tab, in the Name box, type centerline, and then click OK.
  5. Right-click the centerline symbol and select Hide.

   

Now you have a named centerline that you can use to create linear dimensions.

  1. Choose Home tab→Dimension group→Linear.
  2. In the Measurement group, set the Method to Cylindrical, and select the Use Baseline option.
  3. In the Selection bar, in the Name Selection box, type centerline, and then hit Enter. Note: You may have to add the Name Selection box to the Selection bar.
  4. Now select the second object you want to dimension.
  5. Before or after you place the dimension, you will need to remove one of the arrow lines by clearing the Show Arrow Line option in the Settings dialog.

 

Re: Half cylindrical view in drafting NX 9

Valued Contributor
Valued Contributor

Hi all,

Thanks for your replies and help.

 

Thanks,

Yunus M