Exclude Component from section

[rohitagr]

When we create section of an assembly some components we don't want to be sectioned for eg of shaft, bolts, etc.

Is there anyway to do so?
I not only want section lines to be removed but also the whole component to be seen as without sectioning.

 

[FDdesign]

I understand your question but there are 2 different ways to exclude a component from a x-sec:

1. 
   <LI>Exclude a component from the x-sec. You can only do that in drawing mode. When you have your x-sec on the drawing you can exclude component. however,.... the component will still be visible but will be in a non x-sec state. This is not yourwanted result.
   <LI>When you won't see the whole component .... Make a simplified rep in your assembly and set the components that you don't want to see in your x-sec as 'inactive'. When you now show your x-sec AND you are in that specific simplified rep, you won't see that component.</LI>

Kind regards,


Filip Deconinck
Edited by: FDdesign

 

[rohitagr]

Thanks for reply. I want the component to be visible but in unsectioned form. for eg a bolt has a hexagonal head. when we section it in middle it looks as a big rectangle attached to thin rectangle.
I want that even when I do section of the assembly the bolt should be visible as in front view(without section)
I am attaching an autocad view.

View attachment 553

 

[FDdesign]

Ahhh, probably I misunderstood your question .....


If you want tohave the same result as on that autocad view , use solution 1.





Kind regards,


Filip Deconinck

 

[rohitagr]

View attachment 554

I don't want even the first option. I want the component to be without sectioned(cut).

 

[FDdesign]

OK.


After you excluded that 'component' AND after you updated your sheet/drawing view, the hex shape will appear like in the autocad drawing.



Edited by: FDdesign

 

[rvm_22in]

No, you won't get it my Friend!

 

[FDdesign]

Strange statement my friend !! Did you do everything right ?
See picture below. Done in Wildfire 2.0


View attachment 555


Kind Regards,
Filip Deconinck
ProE Support Consultant
Edited by: FDdesign

 

[rohitagr]

FDdesign,
How to do this?

 

[FDdesign]

OK, do the following.
I used a ProE WF2-assembly, called 'engine'. You can download it from http://www.ptc.com/go/handson/models. (I used the file 'Advanced Pro/ENGINEER Hands-On Workshop Models',and in the subdirectory 'Part_Modeling' you will find the assembly 'engine')
I created aplanar Xsec and I've made a drawing with a general view containing a Xsec. The view is set in a 'No Hidden' line display.
View attachment 556
Select the Xsec (it will colored red)
View attachment 557
Click the Right Button Mouse (RMB) and select Properties. The screen be like this:
View attachment 558
Click in the dialog box that you get on the right part of your screen on 'Next Xsec' until the 'glow plug' is selected.
View attachment 559
Click now on 'Xcl Comp' > 'Done' AND update your current sheet 'View' > 'Update' > 'Current Sheet'(You could also just update your drawing view if you want it will get the same result)and you will get the following result:
View attachment 560
You have now a Xsec however the 'glow plug' on top of the engine will not be Xsectioned.
You must use the same technique, in your assembly to get your wanted AutoCad result !!!


Kind regards,
Filip Deconinck
ProE Support Engineer
Edited by: FDdesign

 

[stefanba]

Hi,


I developed a small Pro/TOOLKIT application which allows you to setup rules for components which shall be excluded (like IF partname contains "bolt" THEN exclude). Then the software gives you an additional button in the X-hatch control menu to run all these rules and exclude the specified components from X-hatching. If you are interessted in this toolkit application, send me an E-mail at [email protected]then I can send you this software.


Stefan