If you're working in the Master Model Drawing mode than one of two things have happened, either you've explicitly added the Datum CSYS to the Model Reference Set (it can't happen automatically) or you're using the 'Entire Part' Reference Set.
If you not using the Master Model mode (which you should be) then simply Hide the CSYS before you start adding views to your drawing.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
I am using Master model mode. All my assembly drawings have the Datum CSYS visible by default.
I am not sure about reference set. When working in drafting i right-click the assembly in Assembly Navigator. In "Replace reference set" entire part is selected. Other option is "Empty". If i right-click every individual part in Assembly Navigator all have "MODEL" selected. Is this OK or am i looking in wrong place?
Go to Information -> object and select the datum csys, the report will tell you what part 'owns' the csys. This will give you information to track down the problem.
Go back to the original master part file which you are making the drawing of (this would be the part file below the 'drawing file' you see if you open the Assembly Navigator while in Drafting). Now with the master part file the displayed file, go to...
Format -> Reference Set...
...and if a Model Reference Set exists, select it and see if the CSYS is highlighted along with the rest of the model. If it is, then 'shift-select' it to remove it from the Reference Set and then select the 'Close' button.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Hiding the CSYS (datum csys, I assume) will remove it from the views, but depending on future edits it may pop up again. The best solution is to remove it from the reference set. If you are not able to select it, double check your selection filter; it may be set to 'solid' or 'curve' or something else that is ignoring the CSYS. Change the filter to 'no selection filter' or 'datums' (if it is a datum csys, 'CSYS' if it is a saved csys) and you should be good to go.
What version of NX are you using? I know in version 6 or newer (and possibly version 4 and 5), there is a 'selection' toolbar that is always available. The filter setting may change depending on the command you are in, thanks to dialog memory. It is easy to miss and I have seen it cause much confusion.
I just realized that i was looking at reference sets in drafting and not the master part file. The master part file in my case is the assembly i assume? When im in modeling and looking att reference sets for the assembly there is no Model Reference Set.
Then it's possible that the CSYS is inside one of your components. If not, try Hiding any CSYS opjects that you see while looking at just the Assembly.
BTW, if you found NO 'Model' Reference Set while you were in the Assembly file, that's GOOD NEWS. It indicates that you're using the system properly since we recommend that you NOT create Reference Sets in an Assembly, ONLY in piece parts.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
