NX8.5 sketching and color related question

[jyk1]

Hi,

I've been using NX8.5 with TeamCenter few weeks now and I'm off to good start but I have a few questions:

When sketching for example basic rectangle, I'm used to position it on the sketch using centerlines of the curve. For example in Solid Edge, the dimension tool is able to snap on the midpoint of the line. In NX, I have to draw separate reference line in the middle of the shape, sometimes even in several directions. Is there a way to change this?

And also is there option for changing the decimal separator from point to comma? Because I'll do all the numeral input from the numpad and NX does not accept numpad comma for separator so I have to "fetch" the point from the middle of the keyboard everytime. If I change keyboard layout to American it works but it's not very convenient because I need Finnish layout in everything else. This also a problem in other softwares though..

And one more question about coloring the assemblies in NX:

If I have an assembly with several similar subassemblies. I change the color of the subassembly but the upper assembly does not inherit the coloring from lower assembly. It works if I color the parts separately but it's much faster to color in assembly level. Now I have to color the subassemblies at the top level, each separately. Is there a option for this?

 

[kapmnit123]

Hi jyk1,
I have attached a movie herewith for your last point (specific sub-assembly color).As shown it is very much doable in NX and this change can be reflected at top level assembly also (however i have always restricted myself doing the display properties change at part level only).
I was not able to get the motive behind your second point..decimal seperator (is there any specific reason behind it?)
As far as your first point is concerned (though i have never worked on SE) i feel we hardly require dimensioning wrt a mid point of a line (dimesions need to be referenced with proper part features and not just virtual points lying on any entity.). As far as constraining is concerned then NX allows you to do the constraining wrt the mid point also. Do let me know if there is any use case of yours i am missing.I would be happy to learn new things.
Best Regards
Kapil Sharma

 

[jyk1]

Hi Kapil,

Thanks for the video, that was very helpful.

The motive behind the decimal separator is just speed and user-friendliness. Very often I need to input decimals after the numerals when using CAD ie. 2,5. And numeral input is much faster and easier to do with keyboard numpad and the comma separator works for example in Excel, Solid Edge so I'm used to it. And I know this is country-related thing whether the separator would be comma or dot. But anyway the 'dot' is not conveniently usable on keyboard layout when inputting numerals from numpad and it would be nice if there'd be an option for selecting which to use.

For the midpoint thing. Very often in my work I have for example steel plate on which I need to cut some rectangular shape slots. The slots need to have some play in odd numbers (ie. width 40,4 mm) but still I need to position them by centerpoint. So in ie. SE it's very easy to constrain dimensions on the centerpoint of lines without drawing any "extra" reference lines or calculating some odd numbers.

These are all very minor problems and most of them bugs me because I'm used to work in different method. So I was just wondering if there'd be option for these because in general NX is very customizable.

 

[carlharr]

Hi jyk1,

There is a midpoint constraint in NX which allows you can use to align any selected point with the midpoint of a line (or external edge), projected normal to that line or edge.

It requires selection of one point (i.e. arc centrepoint, line endpoint), and one line to find the midpoint.

If you are trying to "align" two parallel lines midpoint to midpoint, neither of them has a selectable midpoint. So, use the 'point' command and put a point on the midpoint of one of the lines. Afterwards you can use the constraint.

Or alternatively draw a reference line which is very quick with midpoint snap on.

Some screenshots attached.

http://www.jcb.com

NX 7.5 with TC 8.3

 

[jyk1]

Hi carlharr,

I attached a picture of case what I meant. On picture I've placed points on the middle of the line (which was actually faster than drawing the reference line, didn't thought of that, thanks =)

That could be done without any extra work in SE but it's fine, I'll try to adapt different methods .

 

[carlharr]

Hi jyk1, I understand what you mean now.

I think I'd probably do it slightly differently using points on the top edge (attached) or a construction line, but really its much of the same!

Regards, Carl

http://www.jcb.com

NX 7.5 with TC 8.3

 

[cowski]

Re: color of components in the assembly
There is an option to change the color of a body in the assembly and drive that change all the way back to the original part file if you so desire. While in the assembly:
[ol][li]Edit -> object display[/li]
[li]change your selection filter to 'solid body'[/li]
[li]select the body(ies) that you want to change[/li]
[li]expand the 'settings' section of the edit object display dialog[/li]
[li]check both the options (apply to all faces, apply changes to owning part)[/li]
[li]change color as desired[/li]
[li]Ok out of the dialog[/li][/ol]

www.nxjournaling.com

 

[JohnRBaker]

With respect to your creating a Sketched Rectangle constrained the way that you want, you need to create them using the 'From-Center' option and then actually selecting a 'point' to reference, such as the center of an arc or the end of a line. If you just select a screen point, then the rectangle's center-line references are NOT created automatically, as shown in the attached video.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.