thicken outlines

[Crocostimpy]

Where I work we want to make the outlines of the part in our drawing views a heavier line weight than the rest of the lines. So far the only way I've been able to do this is by creating a curve at the intersection of surfaces in the part, changing the lineweight of the curve and putting it on a layer, then showing that layer in the drawing. It starts to get confusing when there are multiple views, with different layers for each view, the intersection not being the same as the silhouette, yada yada. I haven't found any way of selecting the outline in the drawing and changing lineweight.

Is there some other way to do this? Perhaps in the drawing and not the part?

Mike

 

[cowski]

You can change the lineweight of individual curves with a view dependent edit. However, this is far from an elegant solution as you would still be required to pick each curve that makes up the part outline.

My question would be why do you need to do this? Is it required by some drafting standard (or company standard) that you are using? Does it improve some downstream workflow or is it someone's preference that is held over from the pencil & paper days? It may be time to ask if the benefit is worth the extra work.

 

[Crocostimpy]

Because my boss wants it that way. And yes it is a holdover from the days on the board. I tried to dance around the question of whether we really need to do this considering how much of a pain it is, but he was adamant about finding a way to do it because they do it in IDEAS. Personally I don't think it's worth all the hassle, but it's not up to me.

Mike

 

[JohnRBaker]

Can you define exactly what you mean by "the outlines of the part"? Perhaps you can include a .pdf of an example drawing.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[cowski]

Show him how labor intensive that is then suggest that by changing the 'rules' he could claim a cost savings and/or timeline improvement on his accomplishments for the year.

I'm being 1/2 serious and 1/2 cynical.

 

[ewh]

"...because that is the way that we've always done it" seems like a pretty lame reason to me. Are your drawings otherwise done per ASME Y14.5-1994?

When the people fear their government, there is tyranny; when the government fears the people, there is liberty. - [small]Thomas Jefferson [/small]

 

[Crocostimpy]

After poking around in View Dependent Edit again I managed to find how to do it that way. Yes you have to go around and pick every line. Tedious. I guess that's the way they do it in IDEAS too. I used this method on the drawing I'm currently working on and it didn't take a huge amount of time. In the end I think it's better than all of the curves and layers.

John, all our stuff is proprietary, but I threw together a quicky part and drawing. Not sure how obvioous it will be when you look at it. The 'outline' of the view is a heavier weight than the inside horizontal lines. I use the thickest setting for the outlines, and actually created custom lineweights because the default wasn't a big enough difference between the middle one, IMO.

EWH: ASME standards? I dunno. When I got here they gave me an internal standards book and said "This is how we want our drawings to look." It was that way at every previous employer of mine too, now that I think of it. And that goes back a ways!





Mike

 

[JohnRBaker]

I'm sorry but that .pdf file looks like all the curves are the same width. Which do you mean as being the 'outline' curves? Are you talking about the outside edges or profile of the shape?

However, if this shape is indicative of the types of models that you're creating, why not, under the View Style, just set the 'Visible Lines' to Wide and the 'Smooth Edges' to Thin, as I did in the attached picture of an example I built similar to yours.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[Crocostimpy]

Yes I meant the outline curves. What you drew is exactly what I'm trying to do. I didn't try the View Style settings because I didn't know what they meant, and it wasn't obvious when I was looking around through the menus. Rest assured that I'll be playing with them now though! Thanks for the info.

Mike

 

[hudson888]

Try go into the view and try Insert>Curve from Bodies>Extract>Shadow Outline and then just assign those curves to be thick line type. It is very easy, but non-associative and I wouldn't want to have to use it but I don't know of another way.

I very much think that your boss needs to listen to some common sense that this just isn't a good idea in NX. He's making a rod for his own back or maybe pushing an agenda of some kind. At any rate NO is the better answer because this is just going to be a waste of time and money.

Good Luck

Hudson

 

[hudson888]

I stand corrected in NX-5 it seems that the shadow outline is associative, when you make changes and update the view then it will update correctly. Also to make sure that it starts out as a think line and stays that way you should change the object display preferences to thick line type before you create the shadow outline. If you change it belatedly it keeps reverting to its original line type.

QED

Cheers

Hudson

 

[Crocostimpy]

Hudson, I was going to try your suggestion, but I got an error message that said "Invisible hidden line view required". When I checked the Style settings for the view the hidden lines were already set to invisible, so I'm not ure what's going on there. I've tried it on two different drawings so it's not something goofy with the drawing. Any ideas?

Mike

 

[JohnRBaker]

That only works in Modeling and then you must be using true 'Wireframe' display and not the new shader-based scheme which is now the default.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[Xwheelguy]

Mike,

I feel your best bet will be to change your View Preferences default settings like John Baker pointed out earlier. Those settings should control the majority of the model edge displays on your drawings.

The Hidden Lines tab sets the preferences for lines that are hidden.

Visible Lines tab sets the preferences for all visible edges that are not concealed (or Hidden) by other geometry. I believe you will want this set to either Normal or Thick....probably Thick just to make sure you can see a difference without having to zoom in like on your PDF that was attached in a previous post.

Smooth Edge tab sets the preferences for smooth edges, or what I like to refer to as tangent edges. I believe you may wish to set these to Thin, and maybe even add a different line font like Phantom. This might give a person viewing your drawing a sense of a softer transition between surfaces than a Solid line font.

These 3 settings should take care of the majority of what you're wanting, however there will still be instances where you have no choice but to rely on View Dependent Edit. Most of this can be controlled by making sure all tangent edges are in fact tangent. The reason for this is because if you set your Smooth Edge display to a Thin line weight, and the edges aren't tangent, then they will revert to Visible Edge settings and display with a Normal or Thick line weight (depending on how you've got that set).

I would recommend setting up your Customer Defaults to whatever it is that is required so you don't have to do this every time you create a new drawing.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[FXjohn]

I find it easer to set visible lines to a certain color then assign that color a pen thickness. Use the color by width option

 

[Crocostimpy]

NK, the more I think about it the more I'm convinced we're going to have to use a combination of these methods. What we design here are plastic bottles, and while you'd think that our models would be smooth and tangent all over, there are cases where they aren't. Going through View Dependent Edit or extracting curves might be the way to do it in that case. Most could probably benefit by changing the Visible Lines settings though. As usual, there's almost never one method of doing something that works in all situations.

Thanks to all for the suggestions.

Mike

 

[FXjohn]

I would go ahead and just start using a mono line width for awhile and see if anyone even minds. We had a checker at one time who would mark that kind of stuff up but forgot about it once we conspired to hand in plots with no thickness differences at all.

 

[Xwheelguy]

Mike,

Yes, more than likely you will have to use a combination of the View Preferences and then fall back on View Dependent Editing for uncooperative edges.

We use this same method for wheel drawings, with our Wireframe Smooth Edge display in Modeling set to Thin Phantom lines. If a Smooth Edge doesn't appear in Modeling correctly, then we'll know that it probably won't display like we'd prefer in the Drafting view.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[hudson888]

Here's how I did it and this is the ONLY way that I would recommend if you have to do it at all.

Go into DRAFTING add a view. Change the object display preferences I just set it to thick lines. Then pick the view and "Expand Member View" then Insert>Curve from Bodies>Extract>Shadow Outline. You don't need to select anything it just applies itself.

I tested on components and assemblies in NX-5.0.4.1 and it worked fine. I used an isometric view and I changed a couple of things finding that updating the views caused it Shadow Outline to update so I was satisfied that it can be made to work.

You have to go into each of your Drafting views individually, but you don't have to spend all that time messing about in Modelling.

TIP use monochrome display with line widths turned on.

Cheers

Hudson

 

[NXPERSON]

We are on 5.0.5.3

I have our site setup to Plot our drawings with 3 different line weights when using the Plot command. Look for the Color and Width section. Use the Custom Three Widths option. Open the Custom 3 Widths command. Set your line thickness for the Thin, Normal and Thick line charactoristics.

These settings can be predefined in the Customer Defaults, Gateway, Plotting, Widths tab so they will always be preset.

See if this helps.

Cheers

NxPerson