Detailing Diameter's in a Section View. 1

[spagdin]

We are currently running SW 2007 but no matter how many releases there are why haven't solidworks come up with a way to detail a diameter in a section view which applies the diameter symbol automatically. Regardless of the view being a section, why isn't solidworks smart enough to know the face is still a diameter. Has this been sorted in future versions? I know Unigraphics has had this function for years!

 

[fcsuper]

Is this in regards to a section view with the sketch used to form a section line? Or is this a cut made in a model that is then shown in the drawing as a section view?

Also, now are you making the diameter? Is it sketched and cut, or done with hole wizard?

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[fcsuper]

...and which direction are you trying to section?

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[spagdin]

Imagine a circular bar with a bore to keep it simple. I created the sketch and revolved. In the drawing I took a side view and sectioned it to get a view showing the internals. If I then use smart dimension to dimension the O/D or I/D I get the correct size but as a linear dimension (no diameter symbol). This may be a section view but in reality surely solidworks still knows this is a diameter??

 

[fcsuper]

Is SW interprets the dim as a linear, it will not add a diam symbol, even on a diameter. Have you tried bring your dims in from the model and using those on the drawing? If you are looking for short cuts, it doesn't get much shorter than that.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[CorBlimeyLimey]

If you use the Insert > Model Items method to apply the dimensions, the Ø symbol is applied. If you use the regular dimension tool to select the points or lines involved, then a linear dimension will be given.

 

[JMarv]

In theory, when you manually dimension the section view, you're not really dimensioning the diameter. You're dimensioning from one cut (silhouette) edge to another cut (silhouette) edge, where the section line cuts thru the part. If your section line cuts directly through the center of the part, then your edge to edge dimension will be equal to the diameter, but it isn't technically a diameter measurement.

Joe
SW Office 2008 SP5.0
P4 3.0Ghz 3GB
ATI FireGL X1

 

[fcsuper]

JMarv,

In terms of software, you are correct, but I'm not sure that logic holds for real world use. However, you have a point that I will look into in the ASME standard.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[ewh]

ASME Y14.5-1994 does show such an animal as a cylindrical dimension, and goes as far as to state "Where the diameters of a number of concentric cylindrical features are specified, such diameters should be dimensioned in a longitudinal view if practicable" (emphasis mine).
While this does not directly address the issue of a cylindrical section as in the OP, it does address the desirability of cylindrical dimensioning, which is apparently not supported by SW.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[JMarv]

Matt,

I agree that there is a difference between real world use, and how the software interprets this. I guess my post wasn't clear, as I was only trying to describe how the software interprets a dimension applied in this manner.

Joe
SW Office 2008 SP5.0
P4 3.0Ghz 3GB
ATI FireGL X1

 

[spagdin]

It looks like unless you insert model dims then SW just assumes a linear dimension. That's ok, I thought I'd ask as we dimension manually to cylindrical sections regularly and it I seem to have this habit of forgetting to add the diameter symbol! It would be good to have this "semi-intelligence" in SW but I guess I should just remember to put in the dia. symbol!!

Thanks for your help guys.

 

[mjcole]

You could create a Centerline in the View and make it colinear with Temp axis of Hole or use a relations to side plane
The if you dimension to the centerline you can get a double dim. For revolve features this will make a diam symbol but you'll probably need to do that manually in drawing.

You might be able to show in another view and CTRL+Drag to copy it to the section view.

Michael