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Create a 90 degree section cut

Create a 90 degree section cut

Create a 90 degree section cut

(OP)
I need to create a section view (in modeling) only instead of all through but a 90 degree cut(like other cad systems offer). I have an assembly which would like to show the cut half way thru in "X" and half thru in "Y" thus showing 3/4 of the assembly. Is this possible in NX 11?????

thanks

Cj Silver
Tooling Engineer
Live everyday like no one is watching...

RE: Create a 90 degree section cut


I'm also played much with view section to get this 90 degree cut but without succed
I hop someone here can help.

RE: Create a 90 degree section cut

You should look into the details of "Break Out Section View" - I found it a bit picky when I first started using it but it does what you require.

In case the help file isn't very helpful: There are some threads on this forum I found after a brief search. There are also some youtube videos that walk you through it.

ETA: Here's the help page for a version of NX10: https://docs.plm.automation.siemens.com/tdoc/nx/10...

RE: Create a 90 degree section cut

(OP)
Sorry to be SLOW and I have PMI license, in John's example is the PMI example is that created by a sketch? or how is it offset ...by the way that is exactly what I am looking for... just not sure how to do that version

Cj Silver
Tooling Engineer
Live everyday like no one is watching...

RE: Create a 90 degree section cut

(OP)
and how do I subtract the box verses subtract everything not
in the box

Cj Silver
Tooling Engineer
Live everyday like no one is watching...

RE: Create a 90 degree section cut


If I don't wrong I was seen this 1/4 section when an NX representor come to ouer company
and represent this 1/4 section in NX3.

So in which vertion start the PMI ? (is it in NX3 ?)

RE: Create a 90 degree section cut

(OP)
I am in NX 11... I can change the size of the box but the box subtracts everything and so I end up with 1/4 verse the 3/4 that I am looking for? I know I am doing something wrong because of what I see in john's example

Cj Silver
Tooling Engineer
Live everyday like no one is watching...

RE: Create a 90 degree section cut

Sounds like there's something set to 'intersect' rather than 'subtract' in a boolean option somewhere.

I'll have to go through and try that and see what I find - I think John's example looks easier than the 'break out section view' I mentioned earlier, that I currently use.

RE: Create a 90 degree section cut

Using the 'Assembly Cut' method, there is no boolean setting to change, and it works as desired.

Using the 'PMI Section' method, I experienced the same. Everything worked exactly as John explained. For 'Assembly Cut' I had created a 'block' object to do the cutting. Since I already had that block made, when I deleted the 'Assembly Cut' and began the PMI Section, I simply selected the 4 edges of the block as the "Cutter" section curves, and it automatically calculated the limits. I adjusted one end using the grips and set the 'end plane' where I wanted, to create that partial (1/4) section.

All went well in NX 10.0.3.5 - so I'm sorry I can't troubleshoot your error. I didn't even see where I could force it to give me your results.

RE: Create a 90 degree section cut

(OP)
Again sorry for being so slow LOL... the PMI Version is what I am trying to use and I want to cut out 1/4 of a rectangular assy. I understand how to use the assembly cut method but with the PMI version I can create multiple views for the other engineers to use in PowerPoint. John show way but having trouble duplicating it... I can create the cut away but I end up with 1/4 remaining. I am looking to invert that to show 3/4...is this possible?

Cj Silver
Tooling Engineer
Live everyday like no one is watching...

RE: Create a 90 degree section cut

Here's an example I just created. the "before" on the left, and results on the right. Dialog settings; center.

I believe I found your issue. Do you see the "Material Side" button, right under the "Recalculate Limit Values" button? Give it a click. It will appear to do nothing until you hit <OK> to apply changes. But it inverts the boolean operation.


RE: Create a 90 degree section cut

It will appear to do nothing until you hit <OK>
See on the sketch rectangular and when you click
the flip arrows icon you should see a handle arrow
that show the keep volume. Play with the flip
and you will see it
 

RE: Create a 90 degree section cut

ah, subtle. I see. Thanks.

RE: Create a 90 degree section cut

(OP)
this is it and makes sense but I think I am in the wrong command cause I can not find the menu you showed...

Cj Silver
Tooling Engineer
Live everyday like no one is watching...

RE: Create a 90 degree section cut


To see the menu click the start menu and check the PMI (a v in front of it)
then choose the PMI menue and from the drop down menue select section and then section view
and you shoold see the dialog

RE: Create a 90 degree section cut

No you selcted the wrong dialog !
You selected the lighting section view
you should select section view
sory I'm using nx8.5

Go to the step just before selcting this light sec
And simply select the other one.

RE: Create a 90 degree section cut

If you don't find
go to help command and type PMI
And see the list that appeared for something
like pmi section view

RE: Create a 90 degree section cut

Ok sorry in a second look I see that the right
dialog is the correct one
So go to the right dialog (in your picture)

And choose the icon for sketching
and sketch a rectangle and use the extrude prameters
To define the keep remove volume
and then chose the components to operate on

Sorry I'm using nx85 and its difficult to guess
how it in nx11

RE: Create a 90 degree section cut

In nx8.5 the dialog is as your right dialog
But in its top has a select objects command
and in yours I don't see it.

RE: Create a 90 degree section cut

Do you can get the right dialog directly
without using the Left dialog ?

RE: Create a 90 degree section cut

(OP)
Sorry in my screens I see no options for sketch option in NX11...

Cj Silver
Tooling Engineer
Live everyday like no one is watching...

RE: Create a 90 degree section cut

You have but its dimmed
its right near the select curves with the green v
In your picture before the select curves icon

You need someone that use nx11

RE: Create a 90 degree section cut

Its in the red ellipse in your picture.
but I don't know why it is dimmed.

RE: Create a 90 degree section cut


NX8.5 dialog




RE: Create a 90 degree section cut

FYI.


The pre NX11 PMI Section View command is in NX11 called "Section View(Legacy)"
It is not included in the out of the box user interface, nor is it found using
Command Finder. You need to use menu Customize function and search for
"section view" to find it and add it to your current menu.
As "Section View(Legacy)" in NX11 have the same functionality as Section View
command had in NX10, you can use it to, for instance, define a stepped section.

RE: Create a 90 degree section cut

(OP)
OMG Thanks for the help teaching me how and sdeters for explaining why I couldn't find it... but you all did not give up getting me through this

thanks this is why I love this board!!!

Cj Silver

Cj Silver
Tooling Engineer
Live everyday like no one is watching...

RE: Create a 90 degree section cut


I'm happy you got it.
Is the dialogue the same as in nx8.5?
Do you successful to build the 1/4 section ?
I'm also love this board

RE: Create a 90 degree section cut


Hi,

I am happy to found it also.

Do you know whi it was moved ?

Regards
Didier Psaltopoulos
http://www.psi-cad.fr

RE: Create a 90 degree section cut

That's not the first time things moved.

I don't know why. But I think its a software
organization matter.

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