NX 8.5 Drafting issue - Cannot insert drawing views

[Fonzee]

Hi all,

I am not a power user in NX and I am having an issue that I cannot fix. I am using version 8.5 and the problem I am having is creating a Draft from a part that I designed. I selected the Drafting tab to begin creating my drawing and right away I knew something was wrong because on every other drawing that I create there was a light gray dashed outline around my template. This drawing that I am now having the issue with the dashed outline is yellow and when I try to import my drawing views they disappear in the drawing view, but they are visible in the drawing tree. I have tried changing the sheet size as well as the scale on the drawing and nothing seems to be working. Any help would be appreciated. Thanks!!

 

[cowski]

Are you using the master model method (part is a component of the drawing)?

The fact that you are seeing different colors than what you are used to may indicate that this file was started from a different template. You state that the views are "disappearing, but show up in the tree" makes me think that the view is empty with the view border turned off or the default line color is black, blending in with the black background.

Try this: after placing a view, go to Preferences -> Visualization -> color/font -> drawing part settings and check the "monochrome display" setting then press OK. If the views show up, then it was a color setting; if they don't show up we'll have to dig deeper.

www.nxjournaling.com

 

[Fonzee]

Cowski,

I did what you said and it still did not show up. I did add an additional sheet and import my flat pattern and that shows up, but it seems the sheet metal part will not show up. Please let me know if there is anything else that I can try. Thanks!

 

[cowski]

Are you using the master model method?

When you insert a base view, what options are you picking (in particular: part, model view, and arrangement)?

www.nxjournaling.com

 

[Fonzee]

Yes, I am using the master model method. I then select a base view and I have tried different model views. I started by opening my piece part - then switching to Drafting - then I click on "base view" - Placement Method is inferred - Model view is top - scale is 1:8. I then move to the drawing area and select the insertion point at which time it gives me the option to add a projection view and I can see the top of the part at this point. When I finalize the command then everything disappears from the drawing. Even when I have tried the same base insert with the scale set differently it still previews at the same size as the 1;8 scale when I select in the drawing view area. I am puzzled.

 

[JohnRBaker]

Make sure that you don't have a layer scheme in yoru Drawing which is somehow not consistent with your Model.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Fonzee]

John,

I just checked and the layer scheme is consistent between the model and the drawing.

 

[JohnRBaker]

Check you're Preferences -> View -> General and see if you've accidently toggled ON the 'Reference' option.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Fonzee]

That checked out good. I did notice that my representation was Exact (Pre-NX 8.5) so I changed it to Exact and tried it again with the same results.

 

[JohnRBaker]

Without the actual part file and Drawing I don't think that there's much else that anyone could suggest for you to try next.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Toost]

I cannot say anything about the colors or the absence of drawing border, but the picture looks as if you are placing "Reference views"
In your image i see a "x-crossed circle" in the center, this symbol tells that this view is "Reference mode".
A reference view is ( a function that Siemens should hide...hm ) an "inactive view", it's contents will not be visible until you plot.
The purpose is(was) to increase graphics performance by not displaying the contents of the view. - In the old days Unigraphics could not have more than 49 active views on a drawing, the 50:th view would then be set to "Reference mode" ( = inactive / invisible) but it would be plotted.
Edit the Style of the views you have placed and turn off Reference View.
See attached image.

Regards,
Tomas

 

[Fonzee]

Toost,

I tried that yesterday and it was not the issue. I have uploaded the model for all to see and hopefully we can get something figured out. It is frustrating when things like this happen in a software that I am not totally familiar with. Thanks to everyone who has tried to help.

 

[Toost]

The model is on Layer 99.
In your drawing partfile. Delete all views on drawings that exists.
Select Format- Layer settings, make 99 Selectable. ( tick the left box.)
Add new vie to drawing. Should now be ok.


Regards,
Tomas

 

[Fonzee]

Thanks for the information Tomas. This did work for the part that I uploaded, but I have 2 other parts with the same issue and this did not work for them. I will keep trying after I reboot my computer.