Individual part drawings to multi-model drawing, easily? 4

[fighterpilot]

I have an assembly with about 15 detail parts. Each part is an item in Teamcenter and each has it's own detail drawing in the file. The assembly also has it's own individual drawing.

Now, I'm being asked to take all those detail drawings which are standing alone and make them sheets under the assembly drawing. Essentially the assembly details would be on sheet 1, part 1 details on sheet 2, etc....

Since I've detailed everything already is there an easy way to take all that information and stick it as assembly drawing sheets? Or, do I need to start over and detail everything again? If so, how do I go about creating a multi-model drawing?

NX6

Thanks...

--
Fighter Pilot
Manufacturing Engineer

 

[ewh]

DaSalo,
That is interesting about efficiency. Does this include not having a model to work from but only the drawing?

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[fighterpilot]

JohnRBaker said on 22 Jul 11 20:03

"Try setting all the Reference Sets to 'Entire Part' and see if anything shows up. If it does, it sounds like you have a Reference Set problem."

I set everything to "Entire Part" and tried to place a base view of a new model. Result was the same, no object appears in the view.

--
Fighter Pilot
Manufacturing Engineer

 

[fighterpilot]

John,

Forgot to add (and there is no way to edit previous) but this behavior does not occur on every part. My 'standard parts" i.e. parts I did not design, and the top level assembly, will appear if I select them to create a base view.

--
Fighter Pilot
Manufacturing Engineer

 

[looslib]

There is always the trade off of size of drawing versus drawing view scale. E-size drawing and views at 1:4 or C-size drawing and views at 1:8. Scaled down to a B-size printer copy, they both read about the same.

Jeff, not sure what other forum in Eng-Tips would be appropriate. My experience with the tool designers and their drawings was years ago. That company has since moved from using UG/NX as their primary CAD tool for 18 years to Wildfire for 5 years and then sold by the corporate parent and have since switched to CATIA V5.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[fighterpilot]

JohnRBaker,

There are a couple of questions up there for you. Probably got lost in the thread. They are:

"Try setting all the Reference Sets to 'Entire Part' and see if anything shows up. If it does, it sounds like you have a Reference Set problem."

I set everything to "Entire Part" and tried to place a base view of a new model. Result was the same, no object appears in the view. Also, this behavior does not occur on every part. My 'standard parts' i.e. parts I did not design, and the top level assembly, will appear if I select them to create a base view.

--
Fighter Pilot
Manufacturing Engineer

 

[ewh]

I set everything to "Entire Part" and tried to place a base view of a new model.

Are you adding a view of a model which is not a component/sub-component of the drawing?

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[fighterpilot]

ewh,

No, the item is already in the assembly. I've put the assembly drawing on sheet 1 and now want to put the detail parts of the assembly on sheet 2 thru xx.

--
Fighter Pilot
Manufacturing Engineer

 

[DaSalo]

It still sounds to me like a layer visibility problem as John suggested earlier. Are all layers in the assembly and all layers in the components that contain solids set to visible? Are all objects unblanked (shown)? Does anything happen if you place a view and then use the "Layer Visible in View" tool to reset to global (button at bottom of window)? If all of your layers were already visible that shouldn't have any effect but if the view was placed with some layers invisible that will make everything show up.

 

[fighterpilot]

Never in my life have I had what seemed to be the simplest of tasks turn out to be such a cluster. I think all my problems listed above to this point have been traced back to layers and reference sets, but I'm not certain.

Now a new issue/question.

I added sheet 2 to my assembly drawing and then inserted a base view of the component (det-1) of my assembly (a01) I want to start detailing. Why when I add the view of det-1 does it add another det-1 component into my assembly navigator? I don't want to add another component, I just want to detail what is already there.

I'm attaching an image of the structure.



--
Fighter Pilot
Manufacturing Engineer

 

[ewh]

See my post 26 Jul 11 15:39

What I was trying to refer to was not selecting a part different from the drawing file when defining which view you need to place. As long as you accept the default file (the work file), no new parts should be added. The view will be of whatever is in the modeling side of your drawing, not a different part file. I have known users who detail parts by taking views directly from those parts instead of the drawing model, but have always found those difficult to work with.
Is this what is happening?


"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[looslib]

For your det-1 view on sheet 2, add the assembly view to the sheet 2 drawing view. Now use visible-in-view and turn off all layers except that layer which contains det-1. This assumes that your details are placed on separate layers in the assembly or that you brought them into the assembly on their original layer and each model has the solid on a different layer.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[fighterpilot]

ewh,

Maybe I'm lost with the terminology. You asked previsously;

"Are you adding a view of a model which is not a component/sub-component of the drawing? "

and I responded;

"No, the item is already in the assembly. I've put the assembly drawing on sheet 1 and now want to put the detail parts of the assembly on sheet 2 thru xx. "

See my attachment from my 28 Jul 11 9:30 post today? That is what I see in my assembly navigator. When I select Insert/View/Base View I'm presented with a dialog where it says "Loaded Parts". I just select the det-1 part as the one I want to detail. That's when it adds the duplicate item to the navigator but puts what looks like drawing sheet next to it.

--
Fighter Pilot
Manufacturing Engineer

 

[ewh]

Yes, that is what I was alluding to... I apologize at my poor explanation and more so at my misleading/incomplete response of 26 Jul 11 15:39.
Try Ben's advice, segregating the parts by layers, and adding views only from the current work part (the drawing file).

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[fighterpilot]

Ben,

There is no layer which contains det-1, or any other part for that matter.

Didn't/don't you run Pro/E if I remember right? Think how you would do it in Pro/E, that's where my mind is w/r/t doing drawings.

For the most part I don't use layers in UG. Never used them in Pro/E either. Never saw a reason to do so.

--
Fighter Pilot
Manufacturing Engineer

 

[looslib]

I used UG from V3 to NX4. Started with Pro/E at 2001 and am on WF4 now, with WF5 and Creo loaded for evaluation.

What you have to do is think in NX terms, not Pro/E terms. Hard, but the two systems think differently. In one of my training classes for Pro/E was a couple of others who were coming from UG. Every thing they asked was in UG terms and the instructor had a hard time explaining it. About Wednesday when the instructor was out of the room, I told them that they just had to learn to think differently and gave them some quick differences that they could grasp. The rest of the week went easier.

I never use layers in Pro/E but found them very useful in UG/NX. OK, maybe never is too strong as we do have layers setup in our files but I never mess with them.

Your part MUST reside on some layer in NX! In the component file for det-1, the solid was created on a layer, which one? Was det-1 brought into the assembly on the original layer (from the det-1 file) or on the work layer?

As to the view of a detail component in WF, I would switch Drawing Model and then add a new view.
In NX, you add the view and then hide the other components that you don't want to see in that view. Multiple methods to do this in NX: Exploded views requires view setup), Visible-in-View and layer settings and Hide Component in View. There maybe others.

One of the things complicating your drawing is that you have the drawing in the same file as the assembly. In Pro/E you had two separate files, an .asm and a .drw. Changing to a different model for a drawing view didn't add the component again to the assembly file.

Your company really does need to rethink the all-in-one file strategy and use Master Model. It will simplify things a lot!





"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[ewh]

Ben beat me to it. All good advice.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[fighterpilot]

Started on Pro/E version 14 stayed there as machine tool designer/CAD Admin until 2001. Many, many models created in Pro/E, learning it was never this hard.

It appears det-1 is on layer 3. In fact, all of the parts in this assembly are on layer 3 which right now is the work layer. (Keep in mind I'm not that familiar with layers but this is what I think I see.)

I need to do something w/ this because when I add a base view of an existing component it also adds to my quantity of parts when I look at the structure in Teamcenter. I can't have that as it would be confusing to others.

So it appears the way to fix this is to move each component to it's own layer (rename the layer for ease of identification I assume) and then use the visible in layer functionality.

That's seems so, so stupid and such a waste of time. Now I not only have to manage my structure as I add/remove components I need to manage my layers?

It's pointless for me to try to change things here w/r/t UG. We made it and if you understand that statement, you know where I work then.

--
Fighter Pilot
Manufacturing Engineer

 

[ewh]

We made it

Got away from you, heh? ;-)
If you are taking views from the drawing model file and not the individual part files, the structure should not change.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[looslib]

Well your company may have owned it for a while, but it was made before that. If they own it now, then that is a different story.

You will need to separate the components onto individual layers in the assembly file and use ViV to get your details showing in their respective views.

The reason you are geting duplicate items in TC is because you are ading the model to your assembly for the detail view which is being done in your Assembly file. Move the drawing to a separate file and this won't happen.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[fighterpilot]

I had my drawings under each individual component because that's how I would have done it w/ Pro/E. I got b-slapped because "that's not how we've always done it here" and it's not what the tool makers wanted.

I moved one component to layer 50 and then added a base view of my entire assembly on sheet 2. Then I set the ViV to show only layer 50 for this view. I got the one component I wanted in the view and no additional components in the ANT. This is probably what I'll need to do. This will work for a small assembly but I'm not sure what would happen once the number of parts in the assy exceed the number of available layers.

We don't own UG now, you're right. We bought from the original maker.

--
Fighter Pilot
Manufacturing Engineer