Drawing contain assembly or not?

[swale74]

Hello, I've heard two different methods for drawings in NX 6.0.

One method is to create a new drawing file and import drawing views of assembly and components into the drawing. With the assembly open I go to the "File", "New", "Drawing" tab and start on the new print. From here I build my print using "insert", "view".

I've been told that this is not the proper method. We should open a new drawing file and then go to "file", "import" select part and import the main assembly into the drawing file. Not sure what the benefit of this is. My colleague went on to say that all the drawing views should be of the main assemble and if you only want a component view the other items are suppressed in that view. This makes updating the print a nightmare. Which method is the UG preferred method of print creation?

BTW we are running NX 6.0.5.3 with Windows XP Pro.
Thanks

 

[ewh]

Has anyone there had formal training?
I don't think "Import" is a good idea... you will end up with duplicate files that will need to be controlled.
The master model approach is to create your drawing file, and use assemblies to bring the model into the drawing file.
There are several methods of drawing creation from there, but that is the basic start.

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

 

[swale74]

The formal training was a very basic conversion training. We are all I-deas users converting to UG. I-deas library feature took care of all the data management end of things. We are hoping to soon be running Team center and this will help on the data management end of things.

This makes sense to me. Is the benefit of having the model in the drawing file the ability to quickly update the print? Not sure why two separate files are needed for the drawing and the assembly but then the assembly has to also be added to the drawing. I could see then you have a backup of the assembly so if any deletion happened you are not high and dry.

 

[ewh]

There are several advantages to having two separate files, with a few being: control of the model file, if desired (detailer cannot modify model); allowing more than one person to work on it (one on the model, the other on the drawing); reducing file size for down-stream applications.
I am sure others will have more to add.

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

 

[looslib]

Everything in your system should be in sepaarte files.
Your component parts are in one file. Their drawings are in a separate file. If this component is manufactured, the manufacturing information is in its own file. Multiple NC operations on a part, each in its own file.
Moving to the assembly, a new assembly file is created using the components as members. create a new drawing file of this assembly level. Repeat until you have the final assembly.

Reduced file sizes, concurrent work, ease of maintenance on parts, reuseability of components and sub-assemblies are all benefits of using the Master Model approach to design.



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

Ben Loosli

 

[ewh]

What Ben said. ;-)
As to the title of the post, using the Master Model approach means that ALL drawings are in fact assemblies; even single part detail drawings are an assembly of the model file being brought into the drawing file.

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

 

[swale74]

Thanks for the explanation.

 

[sitti]

Sorry for the OFF.
Does anybody know how to use accentuated letters in NX? I am from Hungary, and I should use accentuated letters in drafting, but can't find out how.
Thank you for the help.

Adam

 

[ewh]

You will probably get more results starting a new thread. People who might know what you are looking for may pass this thread by.

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

 

[DMiller01]

Ben,

Use of separate files is going to be a tough sell at my company. I have to become well versed in the benefits for our specific situation. Maybe you can elaborate some on the master model benefits.

But first let me say that we have a small engineering department of about 4 engineers and are running NX in native mode. We usually detail our own parts. We also don't need multiple engineers working on the same parts at the same time. We do use separate files for CAM programming but currently our drawings are in same file with the model.

The items that might apply to us which you mentioned were reuseability. How does master model provide any greater reuseabily functionality?

The other item is smaller files. I'd love smaller files because I struggle with large layouts of multiple pieces of equipment. But it seems that to do work such as adding and constraining components, adding dimensions to a drawing and printing out updated prints, everything has to load anyway.

I don't doubt the value of master modeling but I am failing to connect the dots.

Thanks

I am using 7.5.2.5 NATIVE on Dell with windows XP OS

 

[JohnRBaker]

If you use Drawing Templates there's NO need to do any 'importing' as the Master Model relationships (Drawing files with a single Component of the part you're documenting) are created automatically as you apply the Template to your part/assembly file.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[looslib]

One advantage of separate drawing files from the model is that when used in assemblies, you only pull the model into the next higher assembly. All of the baggage of the drawing are left behind on disk. With the drawing in the same file as your model, you load both drawing and model data into memory.

My point on reuseability is putting each detail in its own file. I have workd at some places where they model the components in the assembly file. If you are using in dividual files this isn't an issue.



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

Ben Loosli

 

[ewh]

Regardless of the current size, does your company plan on future growth? If so, NOW is the time to set efficient proceedures. You really don't want to be trying to fix these problems five years down the road.

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