NX4: Can't change crosshatching style. 1

[tooldeziner]

Hello all,
Does anyone know how to permanently modify a crosshatch AFTER it has been created.
Here's the problem:
After creating a section view containing several members, coincidentally some of the members are at the same angle as the crosshatching, so that the crosshatching is either parallel or perpendicular to the edges of the part. I change the angle of the crosshatch using STYLE. I save the file and close. Upon re-opening the file, I discover that the crosshatch reverted to its previous angle, as if I had never altered it.
I realize that it is possible to change the STYLE of the crosshatch BEFORE creating the view, but sometimes that is unsatisfactory as well, because whatever angle you change it to, all the crosshatch still looks the same. Sometimes it is desirable to have crosshatching represented differently to distinguish the various parts in the view.
IS THERE A WAY TO MODIFY CROSSHATCHING ON THE FLY AND HAVE IT STAY THAT WAY?

Thanks,
'ziner

Peace Through Superior Fire-Power!

 

[JohnRBaker]

Either before or after you edit the Crosshatch angle, select the section view, press MB3 and select 'Style' and select the 'Section' tab and toggle OFF the item labeled 'Assembly Crosshatching'. Assembly Crosshatching is the setting that causes the different regions to be hatched at right-angles to each other and so when you do an update it tries to reapply that 'rule'. If you disable the option, it will no longer try and maintain that scheme.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS
UGS PLM Software
Cypress, CA

http://www.siemens.com/ugs

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

 

[tooldeziner]

Once again, valuable input. Thanks.

BTW, I looked in Customer Defaults to find the toggle for this, to turn it off permanently, but couldn't find it. Is it there?

Thanks for your continuing support,

'ziner

Peace Through Superior Fire-Power!

 

[JohnRBaker]

I'm not sure that you really want to do that. If you turn it off globally, when you section an assembly all of the sectioned areas will have the same crosshatch angle applied to it. That is, there will be no attempt to flip the directions from section to section. You're probably better off letting it work like it is, and then for those few instances where you don't like the automatic results, perform the edit in the manner I wrote about.

However, never say that we didn't provide you with enough rope to hang yourself ;-)

The Customer Default can be found at Drafting -> General -> Standard. Select the standard that you wish to use, then select the buttom labeled 'Customise Standard' and then select View and there is the option that you can toggle OFF.

But just remember, I warned you what would happen if you do toggle it OFF.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS
UGS PLM Software
Cypress, CA

http://www.siemens.com/ugs

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

 

[tooldeziner]

Understood....
The nice thing about toggles is: they go both ways.

Thanks again,

'ziner

Peace Through Superior Fire-Power!

 

[latchescmk]

John:
I asked for this a long time ago, (10 years or so), But is there anything in the works for defining x-hatching as a part or model attribute. I work with assemblies that use multiple materials. Having the hatching co-ordinate to the attributed material would be a nice enhancement.

 

[JohnRBaker]

In UGS NX 2 we introduced an integrated material library mechanism and in NX 4 added automatic attribute assignment (for bill-of-material purposes). Based on this capability, there are now proposals to tie material color and texture (for photo-realistic rendering) to the material assignments. With all of this in place (actually the attributes should do it) I suspect that we have all that we need to go that extra step and link it to drafting as well. Note that we already have a very full plate, particularly the drafting group, for UGS NX 6, but I'll see what we can do about getting this moved to a higher priority.

John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS
UGS PLM Software
Cypress, CA

http://www.siemens.com/ugs

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