Can anyone provide feedback as to the advantages of separating the model file from the drawing file? Does this really improve performance as far as loading components in an assembly? We currently create our drawings within the model file and we've been throwing around the idea of separating the two. I'd like to know if their's any other advantages (cost/time savings) associated with doing so?
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Master Model method 1
- Thread starter grimmy62
- Start date
Wittenborn
Aerospace
One major advantage of separating the drawing file from the 3D part file is that one person can create dimensions, and drawings while another person modifies the 3D model. What you really do is create an assembly, with the 3D object as a part in the drawing file. Then the assembly gets updated automatically when changes are made to the 3D model.
Some companies do not want their draftsmen to be able to change or modify the original 3D model. So they give the draftsmen access to just the drawing files.
If you have tons of drawings in the same file as the 3D object, the files get rather large.
Hope this helps.
Regards,
Grant Wittenborn
Aerospace Engineer
Some companies do not want their draftsmen to be able to change or modify the original 3D model. So they give the draftsmen access to just the drawing files.
If you have tons of drawings in the same file as the 3D object, the files get rather large.
Hope this helps.
Regards,
Grant Wittenborn
Aerospace Engineer
- Thread starter
- #3
Thanks Grant, But if I can't show some sort of cost advantage to separating the model and drawing, then my company will not even consider changing it's current procedures (I wouldn't either).
I do understand that each separated file would have it's own privledges and ownership, but I don't envision the two being worked on at the same time. In most cases, the model is changed prior to the drawing being updated.
I performed a little test to see if having the drawing and model together would impact downstream users as far as performance. I created a new tooling file for example, and added the model to the tooling file with just the model showing in the reference set. I noticed no problems at all, the drawing does not load.
I guess if you start doing this from day one, It would be the way to go, but changing to this method mid-stream doesn't make much sense.
I do understand that each separated file would have it's own privledges and ownership, but I don't envision the two being worked on at the same time. In most cases, the model is changed prior to the drawing being updated.
I performed a little test to see if having the drawing and model together would impact downstream users as far as performance. I created a new tooling file for example, and added the model to the tooling file with just the model showing in the reference set. I noticed no problems at all, the drawing does not load.
I guess if you start doing this from day one, It would be the way to go, but changing to this method mid-stream doesn't make much sense.
Wittenborn
Aerospace
You are absolutely correct. If you have no "rights" issues with different users, then changing your current process doesn't make much sense.
You will only get into file size issues if you are creating hundreds of drawings around large assemblies (i.e. an entire airplane and all its components).
My company is going with the separate file system mainly for book keeping purposes. If someone wants drawing 10002-0056/A, I can go search for that file in my database, and pull up the drawing immediately, rather than have to go find the full 3D model that drawing "might" be in, and find it that way. You really can't find drawings just by looking at 3D part files without actually opening up the file.
Regards,
Grant Wittenborn
Aerospace Engineer
You will only get into file size issues if you are creating hundreds of drawings around large assemblies (i.e. an entire airplane and all its components).
My company is going with the separate file system mainly for book keeping purposes. If someone wants drawing 10002-0056/A, I can go search for that file in my database, and pull up the drawing immediately, rather than have to go find the full 3D model that drawing "might" be in, and find it that way. You really can't find drawings just by looking at 3D part files without actually opening up the file.
Regards,
Grant Wittenborn
Aerospace Engineer
vanishingpoint
Mechanical
We use the Master model method at my company, and from what I understand it is a requirement if you plan to implement or use the Teamcenter/IMAN PDM system. Teamcenter uses different types of dataset objects. UGPART (drawings/specifications) and UGMASTERs (models) are treated differently by the system.
In a "native" UG environment without user restrictions the master model method seems to me to be more complicated, file management-wise.
Ken
In a "native" UG environment without user restrictions the master model method seems to me to be more complicated, file management-wise.
Ken
sfzh,
To create a separate drawing from the model, just create your model in one file and save it. Create a new file for your drawing and bring the first file in as a component.
In NX, if you have drawing templates set up, you can have your model on the screen, grab a template and drag it to the graphics window and UG will open the new file for you, bring in the model as a component and even place the drawing views on your sheet.
"Wildfires are dangerous, hard to control, and economically catastrophic."
Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand
To create a separate drawing from the model, just create your model in one file and save it. Create a new file for your drawing and bring the first file in as a component.
In NX, if you have drawing templates set up, you can have your model on the screen, grab a template and drag it to the graphics window and UG will open the new file for you, bring in the model as a component and even place the drawing views on your sheet.
"Wildfires are dangerous, hard to control, and economically catastrophic."
Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand
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1
- #8
The marster modeling are usefull if you are working with big assembly. The the data size are smaller for the workstation.
If you already have a part file with a drawinng, and want to change it to marster modeling (written for UG18)- do so.:
definition.: filename = the solid part where with the drawing
File - New
In the dialog box ”New Part File” tjek out ”Non-Master Part”
chose the filename - and change it to filename_doc
Ok
chose the filename
Save
set filename to work part
file-export-part
Part Spicifacition Existing
Specify Part - chose filnavn_doc
Drawing Selection - SHT1 - ok
Ok
set filename_doc to work part
save
/niels
If you already have a part file with a drawinng, and want to change it to marster modeling (written for UG18)- do so.:
definition.: filename = the solid part where with the drawing
File - New
In the dialog box ”New Part File” tjek out ”Non-Master Part”
chose the filename - and change it to filename_doc
Ok
chose the filename
Save
set filename to work part
file-export-part
Part Spicifacition Existing
Specify Part - chose filnavn_doc
Drawing Selection - SHT1 - ok
Ok
set filename_doc to work part
save
/niels
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