drawing file structure

[64polara]

Working in drafting in NX9.
Our cad structure is add the component to the drawing shown in the bottom component of the tree in attached file.
the file above it with the drawing format icon was added to the drawing file when the views were placed on the drawing. this is not our practice and also when you go and select the display sheet icon, nothing shows in the model. I understand why.

Several individuals in engineering created the drawings and dimensioned the detail part with this structure.
is there someway we can replace the bad ( not showing component with the correct component and still maintain dimension associativity?
or some associativity or just the views remain on the drawing associated to the correct component (no dwg format icon).
sorry my attachment is distorted, best I could do for the moment.
Any help or thoughts will be appreciated.


Wayne Huseby
Drafting Checker/Drafter
United Technologies Aerospace Systems
Jamestown, ND 58401

 

[cowski]

is there someway we can replace the bad ( not showing component with the correct component and still maintain dimension associativity?

Nope, at least not to the best of my current knowledge (though I'd be glad to be proven wrong here).

The good news is that it shouldn't matter (though I have had a couple of odd problems with such views) and is actually the required workflow if you are going to use PMI with the master model technique.

The bad news is that you might already be using this technique and not know it. Depending on your NX settings, it is possible to bring in a view from the master part file and not have a "drafting component" icon created. In one of your existing drawing files, go to menu -> information -> object and select one of your drafting views. Look for the "part name" listed in the information window; if it lists your part file (instead of your drawing file), the view is really no different from one created by a drafting component.

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[64polara]

Thanks for the input. I didn't think there was a way to replace it. As a drafting checker we look for the correct file structure per our standards so unfortunately it will have to be redone even though useable.

Wayne Huseby
Drafting Checker/Drafter
United Technologies Aerospace Systems
Jamestown, ND 58401

 

[scout67]

This has been a recent problem for our company as well.

Is there a customer preference setting that can be set to default to the "work part" when placing a view?

Also could someone explain the benefits of not using the "add assembly" into modeling, then creating the drawing based on that files modeling views?

By skipping the "add assembly" step into modeling, you have reduced the versatility of the file. You can no longer copy the drawing file, replace the component to a similar part, and re-associate the dimensions. I can't imagine the countless hours I have saved detailing, by re-using existing drawings.

Thank you.
Ken

 

[64polara]

The only benefit I have experienced so far is when creating a drawing for a complex o-ring seal.
I would add the o-ring seal as a component and create a section view of the o-ring.
Then add a view from the model that the o-ring is used in, do a view dependent edit removing all features to only show the o-ring groove so it could be dimensioned to actually manufacture the o-ring based on the groove geometry.

haven't seen any other benefits yet. Maybe someone else out there could share some benefits grabbing views from another model.

Wayne Huseby
Drafting Checker/Drafter
United Technologies Aerospace Systems
Jamestown, ND 58401

 

[cowski]

As always, I caveat a variable with, it works at the moment, don't be surprised if it's removed in the future.

Here's what I keep in my env file to remind what it is and does:

#Siemens' best practice recommendation for creating drawings is to create
#master model drawings. This means the master model resides in one part file
#while the drawing resides in another part file. The drawing file references
#the data in the master model file. Prior to NX 8, when a base view was added
#to the drawing, the referenced view would default to the model view from the
#current drawing file. This is counter to the master model best practice. So
#a change to the base view dialog was made in NX 8 to default to the views in
#the master model. Users should be aware of this change and understand the
#referenced views and geometry are now of the master model and not what is in
#the drawing file. If users want the pre-NX 8 behavior, they can change the
#part option to use the current drawing file and not the master model file or if
#they wish to have this as the default for the system they can set the
#environment variable:
NX_MASTER_MODEL_DWNG_DEFAULT_TO_ROOT_PART=1

source:
thread561-381445

If your corporate standard is to use the views from the drawing file, you could try out the environment variable mentioned to make it the default. I don't think the variable will force the drawing view to be used, the user can probably still specify a view from a different file.

www.nxjournaling.com

 

[cowski]

As to why one would want to use these views?
[ul]
[li]If you use model based PMI, you pretty much need to use these views to show the PMI on the drawing.[/li]
[li]You can add reference geometry to the drawing without adding an assembly component (as in the o-ring example above). Also, drafting components do not add to the parts list; so the reference stuff won't show up in the parts list.[/li]
[li]I've heard that toolmakers like to detail several individual parts on the assembly drawing. Using drafting component views would be an easy way to get a view of an individual component and only that component (no need to hide other components from the assembly or use layer visible in view to get what you want). I would imagine that toolmakers love these views.[/li]
[/ul]

Still, I avoid them whenever I can. I've seen some strange behavior/errors with these views and I don't fully trust them.

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