Drawing master/model 2

[MickyV007]

Dear all,

is there a way that i can copy a view plus dimensions from a drawing (conventional) to a sheet (master/model). I tried copy/paste but that doesn't work.

For example : having 3 drawing sheets in model X, then I make acc. to the master/model principal X-110-01 drawing sheet and X-190-01 and X-190-02. Instead of importing all the views / section views, .... again and adding dimensions to it, I would like to copy it from the drawings in model X to the corresponding drawing sheet(master/model).

I know this works in the conventional way of working through Edit --> View --> Move/Copy view...

Thanks in advance,

best regards,

Michaël

 

[hudson888]

If your file isn't in master model concept then it doesn't matter what you do the dimensions and anything else associative IS going to fall over when you separate one from the other. However if you wanted to do so then create the underlying component from the assembly by using the create assembly function. Your dimensions may need to be reattached but it should at least be easier this way.

Now if you just want to separate the drawings into three different files the solution seems even simpler. Once you have done the above you could simply make three copies of the complete drawing by renaming the files and then delete the unwanted sheets from each.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[MickyV007]

Thanks Hudson for the reply,

but still missing something, see att. file. When working with TCE its not possible to create the drawing with the same part name (what you suggested was something like X-110-01,...) but the you got three seperate parts. I want to create the drawing(s) as a specification under the part.

Thus copying the views from the conventional drawings to the specifications and then deleting the drawings in the part afterwards.

Best regards,

Michaël

 

[joycejo]

If you have a drawing in a part file and you want to switch to the master model approach use file Export. Select the Drawing Selection and choose the sheet to export.

You will then be given a choice to add the part as a component of the drawing file. This will keep the dimensions associative. If you have multiple sheets you can create a separate assembly for each drawing.



John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO

http://www.myigetit.com

NX3,4,5,6 Solid Works, Pro/e, Solid Edge

 

[MickyV007]

Thanks John,

that was exactly was I was looking for.

Best regards,

Michaël

 

[hudson888]

I guess you really ought to have stated your version and that you were using Teamcenter earlier.

I'm still not really sure if you want one NX part file for the drawing or three. Since in NX the part lives under the drawing and not the other way around I can assume you're asking to have the part or assembly with the drawing and perhaps each sheet separately collected under the same Item Master within the Teamcenter database?

It may be possible for your TCE admin to help to manipulate the system in such a way as to get this to work for you. I was writing more or less assuming that you might have been working in native.

I can't see the drafting content of your drawing but if it is just one drawing with A4 sheets there can't be enough content to justify the time that it would take to re-organise the data. In that case I might cut my losses re-create the drafting under a new structure.

If on the other hand if this is about maintaining a quantity of legacy data then I suggest that you get a hold of your NX sales people and have them put you in contact with some Teamcenter assistance because that is going to be the tricky part. What I told you above above structuring master model drafting in NX is pretty much it and beyond that I hope you'll allow that I haven't got a clue about your naming convention anyway.



Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[MickyV007]

Hudson,

sorry for not mentioning the NX and TCE version (btw NX 4.0.4.2 and TCE V9.1.3.8) but the solution John provided worked perfect for me. Rather than switching to TCE and
manipulate the system there I got what I wanted via NX manager.
Indeed it would be not worth the effort for 1 A4 drawing, but sometimes we got AO with lets say about 500 dimensions and tolerances which in this case would be time consuming for us to create manualy a specification and put all the dimensions on it.

The file export drawing method has created 3 seperate specifications under the Item master.

Anyway thanks for the effort.

Greetings,

Michaël.

 

[hudson888]

Perfect Good to know!

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum