Dimensioning a free-hand revolved base

[jackosieves]

Hi all, I free-handed a bullet shaped part by using the spline tool and some lines and then revolved it around the center line. I am left with a part that very much resembles what I want it to. Is there any way that I can dimension my splines? I just need a few of the angles. Thanks for any advice.

 

[CorBlimeyLimey]

You can add linear dimension to the points of the spline.

For angles you may have to add tangential construction lines at the points, and dimension to those.

 

[jackosieves]

Yeah, I ended up adding tangential lines and getting angles that way. I was just wondering if there were and easier/simpler way. Thanks for the reply though. Cheers.

 

[Theophilus]

Out of curiosity, why the desire to dimension a spline? Is this for transferring from 3D to 2D for fabrication? (I ask because I do lots of work with curvy stuff in 3D and simply leave it in that format to get injection mold tooling, etc.)



Jeff Mowry

http://www.industrialdesignhaus.com

A people governed by fear cannot value freedom.

 

[Gurjjeet]

Hi Jacko

try this after doing all other relations & the dimensions

1. right click on spline & select "show spline handles"

2. with smart dimension tool on, select spline & click on the diamond shape point on the handle & select any reference hor/ver line & it will give you the angle.

3. Now repeat the step but this time click on the (any of the two) outer most round point of the handle & it will give you a ordinate looking dimension which is handle length(or something)

4. Repeat this on all handles & also dimension the points, this will give you a BLACK spline.

 

[jackosieves]

The reason I asked is because I am transferring from 3D to 2D so that we can send it off to the plastics guys for fabrication. Thanks for all of the help and I'll remember the "show spline handles" for future projects. That should help out some here and there.

 

[fcsuper]

If your manufacturer can produce your part by using the model in some way, you can declare the model BASIC and apply a common profile tolerance to the its entire form (perhaps using ALL OVER).

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper

 

[NomLaser]

I just ran a test on a simple part and if you turn on Sketches in your drawing and in the feature tree for the view you will need to show the sketch that has the spline. You can now mouse over each handle and dimension to it. Is this what you were looking for?