HOW TO MAKE A DRAWING OUT OF A PART FILE

[CADWHORE]

I AM TRYING TO MAKE A PART DRAWING, I CLICK THE DRAFTING BUTTON AND IT ASKS FOR A SHEET SIZE, WHICH IS FINE AND DANDY, BUT I WOULD LIKE TO USE THE TEMPLATES THAT ARE INCLUDED WITH NX4, OR FURTHER DOWN THE LINE SOME CUSTOM TEMPLATES. I CAN CLICK ON THE TEMPLATES ON RESOURCE BAR, BUT IT MAKES A NEW ASSEMBLY FILE OUT MY PART FILE, WHICH IS NOT WHAT I WANT. ANY IDEAS ON HOW TO GET THE PART AND ITS DRAWING IN ONE FILE USING THE STANDARD TEMPLATES???
THANKS

 

[Shadowspawn]

Yes, it is possible to do what you want, but it is time consumsing and a pain in the arse. More importantly, it simple does NOT follow the Master Model concept, which really is important. Why do you want the drawing in the same file as the model? Please explain...

Regards,
SS
CAD should pay for itself, shouldn't it?

 

[CADWHORE]

A co-worker said that this is the way that NX4 does its drawings. I am used to having a seperate part file and a seperate drawing file. When I hit the template button on the resource bar is it creating another part file, or does it create a new assy with the only the part in it?? If you could explain how the drafting side of NX4 is suppose to work in this regard it would be great, thanks.

 

[ewh]

If you really don't want to use the master model proceedure (not recommended), you can import the template file into the drawing space of your model.

 

[CADWHORE]

ewh,

How would I go about doing this? And what is the master model proceedure you guys are talking about? I can already tell that some like it and some don't care for it.

 

[JohnRBaker]

Just so that you know, there is NO separate 'Drawing' file. All NX files are PART files. But don't worry, everything you would expect to be able to do with a 'drawing' file you can do with a 'part' file. So the fact that your part becomes a single-level assembly when you use a template to make a drawing is what you want if you're already used to having your parts in one file and you drawing in another.


John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

http://www.plmworld.org/museum/

 

[phillpd]

It's definitely beneficial to have the drawing file independent of the part (model) file. The Master Model is effectively ...

Part File -> Assembly File -> Drawing File

Specialty Engineered Automation

http://www.sea4ug.com

 

[CADWHORE]

So if I understand this correctly, start with a part file, insert it into a template, it creates a new assembly file that contains the original part file. The new assembly also contains the drawing file, but the drawing is of the assembly file and not the part file. So if you modify the part file, the assembly is updated, then the drawing is updated. So for every part you will have the part file, and an assembly file.

When I am building up a top level assembly what do I use for the parts in this new assembly? Do I use the original part file, or the new assembly file?

Thanks for all the insight, it is saving me a lot of time.

 

[JohnRBaker]

You use the original part file. Remember, just like there is NO special 'drawing' file, there is NO special 'assembly' file. They are are ALL 'part' files. It's just what you do with them and what sort of data you include in them that makes them 'different'.

As for your preception as to what's happening when you make a drawing using a template, you've got it pretty down cold. Just use it that way and I think you will be getting exactly what you want and need.



John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

http://www.plmworld.org/museum/

 

[boldfish]

It's definitely beneficial to have the drawing file independent of the part (model) file.

Why is it beneficial? Can anyone list these benefits?
What about disadvantages to creating the drawing within the part file? Why is this not a good idea?

 

[phillpd]

That's basically the recommended way of working with UG/NX. Hence when you use a drafting template, it creates a parent file to the one you have active. Single part files just carry a lot of overheads. If I'm an NC programmer, then all I want is the model, probably not the assembly, or the drawing.

I guess it depends on the size of your company, as to the benefits. It certainly promotes the use of simultaneous, or concurrent engineering. That is, you can have multiple disciplines working on a project (or product) at one time.

Even NC programmers should ideally consider the use of an assembly file, so that they only have a reference to the product being manufactured.

Specialty Engineered Automation

http://www.sea4ug.com

 

[mjcole]

Most other programs Inventor, Solid Works, Pro/E, Alibre all can create a drawing separate from a part file but still have it linked and be able to change the model from the drawing. They also usually have their own extensions like .drw or .slddrw or .sldprt and you dont have to assemble them in. UG started out like Catia with both the drawing and part in one file.

I don't know why UG hasn't put this type of functionality as all other systems have. I guess if you enjoy purple dimensions or getting paid by the hour then Master Model is for you. It does make more sense the way other systems do it and you can switch items to other views or have views that remain associated to each other.

I hope UG has addressed some of these issues in newer releases of NX. Also most systems create Cross Sections that are tied to planes so you can orient them properly and change their position if you so choose. I had some fun showing a co-worker how to create the section used to create the geometry for a sweep shown in the drawing that had no ties to the actual position of the cross section.

Usually one good reason for using master model is you can work on the drawing and the part simultaneous ly so you can have the Drafting done overseas to keep costs down which I'm not really a fan of.

And a question for John wouldn't it be nice if you could use set views from the part in the drawing file and not have to set up the same views in the Drafting model when you assemble the other part file?

Michael

 

[JohnRBaker]

Basically all we have done with NX is to NOT hide how we link the Drawing to the Part file. From our point of view, we already had a perfectly good mechanism to link one file to another file (to create assemblies) so why NOT use that same technology over and over again ('standardization' and 'reuse' play a role in software development as well).

As for using the views as defined in the original part file on a drawing, starting with NX 4, when you add a view to a drawing and you're given the choice as to which 'view' to place, when you pop-up the list of available views, those who's names are precedded by an '*' are the views FROM the original part file. Those without the '*' are the VIEWS as defined in the current (assembly) file.


John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

http://www.plmworld.org/museum/

 

[DavidTolsma]

Benefits of Master model....

- Smaller individual files
- More then one person can open the files at a time and work on them (a drafter, designer, FEA, etc)
- Control who can see the drawings
- Easier to control what is visible by using reference sets



-Dave

http://plmwiki.com

http://groups.google.com/group/NX_CAX/