Is there a step-by-step process for creating a break out section view? 3

[Mandrill22]

I'm running NX 6.0. The help in NX is useless in this case.

I'm selecting what it asks me to and it's just not doing anything. OK is grayed out.

 

[jerry1423]

There was a video out there someplace showing break-out section steps, but I don't remember where it was.
If you can access YouTube.com at work maybe check there.

 

[cowski]

Perhaps one of these threads will help:
thread561-280462
thread561-100123

http://www.nxjournaling.com

 

[Toost]

It's not that difficult once one has done it once
Start by making the view where you want the breakout view the active sketch view, draw some curve ( Spline) around the area. Finish the sketch and start the breakout section view.
toggle "Create" mode.
pick the view to section, next button:
pick the depth of the cut ( imagine the area that you enclose will be extruded from this pick, i.e if you have a second projected view you can pick in there to indicate the depth of the cut.)
Next button
( this will display the normal direction of the section view, unless you are doing something special, just click the next button
and select the curve that will enclose the area.
IF the curve-s is closed ( encloses an area)press Apply
If the curves are open ( such as a single s-shaped Spline) - click the last button "Modify boundary curves", you can then click-drag the small arcs that appear to form the area that you desire to cut. If you drag an arc to an endpoint it will disappear.

Regards,
Tomas

 

[DaSalo]

The most confusing thing for me when I first started using this tool was the step where you define the base point (Toost refers to this as "Depth of Cut" in his post). As he correctly points out you can use another view on the drafting sheet to choose this point.

I frequently use this tool to show a tooling ball that I need for dimensioning that is hidden behind some other component. I almost always have another view somewhere on the sheet where I can see the tooling ball in true shape from the top. In this other view I select a quadrant point on the shoulder of the tooling ball. This causes the breakout to begin right on the front of the tooling ball so everything that could be interfering is cut away but the tooling ball itself is not sectioned.

It took me a bit to figure out that you could use the other views on the sheet to accurately define this base point.

NX 7.5.5.4 mp01, NX 8.0.1.5
Tecnomatix Quality 8.0.1.3
PC-DMIS 2011 MR1

 

[bruwel]

The most annoying problem is that there is a command requirement that does not appear. After you pick the view, create the boundary et al. There is no clue that you have to pick anything else. The icon to select the sectioned component never highlights.

 

[Toost]

Bruwel, - I dont get this, what is it you are missing / what icon never highlights ?
I do agree that it is a bit confusing/ annoying that one needs to know / create the section curves ( in the view) before entering the Breakout section dialog. I assume that most breakout boundaries are spline shapes and then the regular spline command could have had a "shortcut" in the breakout section dialog.

Regards,
Tomas

 

[Jezovuk]

Hello! I have one question concerning "Break out section view".
I manage to create it's boundary curve (circle) using "Lines and arcs" toolbar.
There are multiple options to create straight lines, circles and rectangles but I can't find a single one to create a SPLINE. How can i draw a spline using Lines and circles?

 

[jerry1423]

Jezovuk, what version of NX are you on?

 

[JohnRBaker]

Why not create a Sketch containing a Spline in the view in which you wish to create your Break-Out view in?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Jezovuk]

Sorry for untimely answer.
Jerry, i'm using NX 8.0.
John, when i create a spline in non expanded view, previous to start of "Break out section" command, the spline is not selectable in parameter selection.
When i go to expanded view, spline command is not selectable.

 

[Toost]

Jezovuk, Exit out from all dialogs in NX, then use Information - object- select the spline and hit ok.
In the listing window you can then read what view the spline is view dependent in,... - In case it is view dependent om the drawing sheet, the text reads "Resides on drawing Sheet x"
In case it is view dep in one of the views, it reads "View Dependent In xxx@xxx"

- The most common (?) mistake is that the curve is not view dependent in the specific view that is should cut but on the drawing sheet.

If the Information Object cannot select the curve either, you have probably messed around with "layers visible in view" .

Regards,
Tomas

 

[Jezovuk]

Yes, for spline that is not selectable, it says "Resides on drawing Sheet 1" .

How can i make it "View dependent"?

 

[DaSalo]

You need to make the view in which you want the break-out section the "Active sketch view". Right click on the view in the tree and select "active sketch view" or right click on the view border and make the selection. Now sketch your spline in the view and it will be view dependent relative to that view. I will now be selectable when you try to create the break-out in that view. If you want to create a break-out in a different view you will need to make that new view the "active sketch view" and so on...

CATIA V5 R20
PC-DMIS 2011 MR1

 

[Jezovuk]

Yes, that is it.
That You DaSalo, Toost, John and Jerry.

 

[wavesurfer77]

Thank you This was very good.
I had trouble with break out section.

/Håkan