NX 7.5 - Colours in drafting

[milancz]

Hi,
we´ve upgraded NX 7.0 to NX 7.5.2.5 MP2, PC with WIN7.

Everything has seemed to be OK.But now I´ve found out a problem with colours in drawing created in drafting NX7.5.

If I open old drawing (made in NX7.0)colours are correct (dimensions - brown, outline lines of objects in views are blue and so on).Colours all entities can be modified.

If I create a new drawing in NX 7.5 all entities are black (dimensions, new curves, outline lines of parts in views....)and they can´t be modified.
I mark the entity, use "EDIT DISPLAY..",pick desire new colour (blue), OK. The entity is black all the time.

If I listed information of the entity the information says that the colour is blue (however on screen is black).
In Preference Color Palette seems to be set "Grey palette".Even if I change the palette to another, Grey palette returns.

Please, any ideas what to do, what set up to be able to use color in drafting? Black and white drawing on screen is very confused.

Thanks a lot.

 

[Arkance/PhoeNX]

Right click on the drawing fold in the part navigator and you should be able to turn off monochrome view of drawings.

Anthony Galante
Senior Support Engineer

NX4.0.4MP10, NX5.0.0->5.0.6, NX6.0.0->NX6.0.5, NX7.0.0->NX7.0.1 & NX7.5.0.32-> NX7.5.2.5

 

[milancz]

Thank for your solution.Now it is all OK.

I very appreciate your advice and it is seemed that great problem (for me) can have a simple solution.Only someone must exist who knows it.

 

[JohnRBaker]

Open your Part file and go to...

Preferences -> Visualization -> Color

...and in the section of the dialog labeled 'Drawing Part Settings', toggle the 'Monochrome Display' option OFF.

Note that this is a 'Part specific' setting which means that you will need to open all of your NX 7.5 created drawings and change this setting. And to prevent this from being in effect on your future drawings you will also need to go to...

Customer Defaults -> Gateway -> Visualization -> Color Settings

...and toggle this option OFF there as well. Also, if you're using a Drawing template, you will also need to open the original template masters and change this setting there as well.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

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

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

 

[milancz]

Hello,

I have made set up ,as mentioned above (by Mr.Baker), "Preference->Visualization->Color....." and "File->Utilities->Customer defaults->Gateway......", shut down NX and start NX again.

I opened new part and I checked settings I made, then setting in section of "Customer Defaults....." is OK but in section "Preference->Visualization....." is ticked "Monochrome" at drawing part all the time.It causes that drawing is black and white.What is wrong in my setting?

Of course, it is possible to correct it by means of mentioned advice above (by NAMDACI45).

 

[JohnRBaker]

Nothing is wrong with your settings, just that the Customer Default settings are 'Part' specific, meaning that they will only effect NEW part files created AFTER you make the Customer Default changes. For those parts which you've already created, you will need to toggle this setting OFF on a Part file by Part file basis using the Visualization Preferences and then saving the files.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

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

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

 

[milancz]

Ok.
I might express incorretly.I meant "opened new part" as "created new part".

I have made the both recommended settings (recommended in the past}.

Now I am going to create new part and its drawing (I suppose that the new created drawig to be right in color).

My steps:

start NX
new part-model-ok
feature-extrude-block-ok
start-drafting
standard size, A4, scale 1:1, ok
placed views
and all is monochrome (black and white)

After inspection settings: in "Gateway-Visualization....is monochrome unticked
in "preference-visualization is monochrome ticked)

 

[Arkance/PhoeNX]

milancz, when you go file-> new and select a modeling or drafting part, they do not read the default from customer defaults because they are already set. If instead you select the blank file type from the bottom of the file -> new dialog you will find hat it will follow the customer default.

To change the others you need to go into c:\program files\ugs\ugs nx 7.5\ugii\templates (or wherever you installed nx to).

In that folder are the part files that are used for the file -> new dialog. Open the right file, change the preference (not the customer default) and then save the file. This will then set the file to your preferred option.

Then when you create a new file it will read from the modified file and use your preference.

Anthony Galante
Senior Support Engineer

NX4.0.4MP10, NX5.0.0->5.0.6, NX6.0.0->NX6.0.5, NX7.0.0->NX7.0.1 & NX7.5.0.32-> NX7.5.2.5, Beta NX8.0.0.15

 

[JohnRBaker]

Tony is correct. I should have mentioned that your 'template' parts will also need to be updated before they will behave as you wish them to.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

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

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