Half of my dimensions are light grey and the other half are black! 1

[sixmillionways]

Hi, does anyone know why half my dimensions on my drawings seem to come out light grey and half of them black? I can't seem to find a link between them and it makes my drawings look very strange...

 

[sixmillionways]

I have solved this, they are driven and driving dimensions. Changing both their properties in tools-options-colours to black solved my problem.

 

[gwubs]

We also set driven dimensions to black. It may be helpful in sketches to add the word DRIVEN to dimensions, so that it is clear which are driving, and which are driven. My earliest drafting instructors drilled it into us that DRAWINGS ARE BLACK - not grey.

 

[SBaugh]

True, but if they are black that indicates that you can change the dimensions from the drawing and it will reflect back in the model. The gray ones will not because they are reference. If you change the color to show all reference and driving dims to black, then you will not be able to tell which ones are driving the model and which ones are not. So the true fix is to build your models and place dimensions on and in the sketches to reflect what you want in the final drawing. This away you don't have to add a bunch of reference dimensions.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[matherjd]

As long as you print black why worry about gray on the screen - seems like you are loosing important information if you set reference dimensions to display black.

Autodesk Inventor Certified Expert
Certified SolidWorks Professional

 

[MadMango]

Actually, Scott has the right idea. It seems if your sketches in the model are properly defined, when you insert your dims from the model, you won't have to insert any reference (grey) dims, unless they actually are reference dims.

"Art without engineering is dreaming; Engineering without art is calculating."

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[Heckler]

So the true fix is to build your models and place dimensions on and in the sketches to reflect what you want in the final drawing. This away you don't have to add a bunch of reference dimensions.

Building your models this way will allow you to experience the true bidirectional capabilities of SWx. Because you can edit those dimensions in the drawings. I realize their are some complex models that will not allow this due geometry constraints. But really why not do it....

I get really frustrated when I see our drafters putting on dimensions in the drawing verses using the dimensions that define the solid model.

Heckler
Sr. Mechanical Engineer
SWx 2007 SP 3.0 & Pro/E 2001
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[CorBlimeyLimey]

I agree also ... If you dimension the drawing manually, you are effectively dimensioning the same thing twice. Not very efficient.

The tolerances should also be set at the models sketch stage so that they too propagate to the drawing.

 

[SBaugh]

You are Right Heckler! There are going to be some things that cannot be defined in the model. but I would only say about 10% or less can not be done easily in SW sketches/features. But if its only 10% then the users should build their models using the most efficient process there is.

Best Regards everyone!

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[sixmillionways]

Interesting discussion, I have never utilised the ability to actually dimension the solid model as I create it in the 3D part view, but will give this method a go next time I create a new part.

Thank you all for your input!