Assigning layers to edge types 2

[montagnamike]

I'm using SW 03 and am trying to assign a layer to an edge type to produce detail drawings on which I can turn the hidden details etc on and off and so that they are assigned a particular line type and colour (just like you would in AutoCAD. Is there anyway to do this and if so how? Thanks,

Mike

 

[ctopher]

What do you mean "edge type"? Remember, this isn't ACAD ... different thinking.
I'm not clear on your question.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-05)

 

[J-C]

Well, you can control the color of hidden lines under Tools/Options/colors. As for layers and model edges, I think you are thinking a little too much in the Autocad frame of mind....as master Yoda has said..".you must unlearn what you have learned". Each view has it's own settings controlling display of hidden lines and such...though the new version of Solidworks will link some views to it's parent view for this setting so you don't have to toggle so many.

For what reason would this be necessary? I understand in Autocad as you are designing in 2d and may want to turn stuff off....but in 3d, you do the same with the displays (Wireframe, shaded, etc). Maybe elaborate on what you are trying to accomplish.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP4.0 on WinXP SP2

 

[montagnamike]

When you're detail a drawing, the edges of the model are shown as different edge types - e.g. visible, hidden etc. right? So basically I'm trying to work out an automated way of making this edges appear as different colours according to how they are shown on the detail drawing - for example a visible edge would be green, a hidden would be red, centremarks purple etc. Obviously you could go through and assign a colour individually to each line, but I'm hoping that there is an easier way than this, that could be applied as a template before each model is imported from the part window. Or can you only apply layers to a whole part?

 

[smcadman]

Tools > Options > Colors > System Colors
Drawings, Hidden Model Edges
Drawings, Visible Model Edges

Flores
SW06 SP4.1

 

[ctopher]

Ah, I see. Flores is correct.
But, in the 2D world I can see using the different colors. In the 3D world, no need for it.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-05)

 

[montagnamike]

Thanks Flores - thats sport on. Its only so that we stick as closely to the company standard as possible... not a proper reason

 

[J-C]

Also, you can create layers that mimic your Autocad layers regarding color and linetypes and put stuff like notes, dimensions, center marks, etc. on them. You just can't put parts of the model like edges on layers.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP4.0 on WinXP SP2

 

[wgchere]

Its only so that we stick as closely to the company standard as possible

It's time for your company to change their standard. Before AutoCAD no one drew in colors, except an occasional block letter in yellow so it reproduced dark on a blueprint (that's how old that color scheme was). AutoCAD came along and used colors and layers to help organize the lines. But we still plotted drawings in Black and White--it was purely an organizational tool. Now your company is using a more advanced generation of CAD. SWx is smart enough to manage all the different entities on its own, using Annotations Fonts and Line Fonts in the Options window. Swx uses colors too, but for different purposes. I work with a guy who uses layers on everything--for example, all his text is on a DIM layer and it's all green, so I can never tell when dims or text is selected because he uses the selection color for his layer color! And if he forgets to change his layer, some of his entities have the wrong characteristics (line weight, line type, etc.) What a monumental waste of time. SWx manages this stuff for you--use the power of the software. "Use the force, Luke!"

 

[peichbauer]

Why would someone want to use different colors? Because we are not all color blind. When I detail a complicated piece of tooling the drawing can become quite cramped and dense with lines of all different types. With colors you can easily, visually, sort out what is an object line and what is a dimension extension line for example. If we were to follow along with that line of thinking that we don't need color on our drawings then why don't you go back to a monochrome monitor??? No? I didn't think so.
Let's think back to old AutoCAD for a second. If we were to bring up two identical customer part drawings (say an automotive part) and one was all white lines, while the other had a different color for each linetype, which do you think would be easier to read?
We do have a couple of guys in our office that are slightly color blind, but there is no reason to make the rest of us that way. This seems like it should be an easy thing for such an accomplished software to be able to do.

Phil

 

[J-C]

Solidworks does colors fine if you want them. You can tell the drawing what default color the model edges should be and a different color for hidden lines. You can specify a color for dimensions (Driving, Driven, and dangling). You can set colors for annotations and for various other entites. And those are set as system options.

On top of that, if you choose, you can create layers and put objects on the layers which override the system color. You can also use the "Line Format" toolbar and further color objects which overrides layer colors.

We have our titleblock in blue, model edges are black, hidden lines are violet, dimensions are gray, and notes are green.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP5.0 on WinXP SP2

 

[peichbauer]

Are you speaking about after you export to .dwg? Or, when working in the 2D portion in SWX? While working in SWX is what I'm concerned about. And i've found where to change the color of the hidden lines under System Options, Colors. But I don't see an option there to control the color of the dimensions or centerlines, etc. in the drawing.
Am I missing something?

Phil

 

[CorBlimeyLimey]

The system option colours also control;
Dimensions, Imported (Driving)
Dimensions, Non Imported (Driven)
Dimensions, Dangling
Dimensions, Not Marked for Drawing
Dimensions, Controlled by Design Table

I'm not sure about centrelines, centremarks, points though.

 

[peichbauer]

None of those seem to control dimension color on the 2D drawing. Keep in mind that I am not importing dimensions directly from the model, instead applying them one at a time.

 

[ctopher]

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

 

[J-C]

Bring up the line format toolbar....there is a button to toggle color between system and user.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP5.0 on WinXP SP2

 

[CorBlimeyLimey]

peichbauer ... Those options do control the drawing dimension colours if you toggle the Color Display Mode button in the Line Format toolbar

If you are manually placing dimensions then you will have to use the Line Format toolbar and/or the Layers toolbar.

 

[smcadman]

All of our lines on our drawings are black, but our dimensions are a dark red and our text is a dark blue. We print our line drawings in color, so it adds to the clarity of the drawing.

You might want to check out a macro written by Handleman. It automatically puts all dimensions on a dims layer and all other text on a text layer.

Dimension color macro

http://www.eng-tips.com/viewthread.cfm?qid=166740&page=1

SW07 SP1.0

Flores

 

[ctopher]

The macro is good. I also suggest making all your dwg templates with the layers you want.

Chris
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)