I am probably overlooking something obvious but when I try to dimension and elipse in drawing page it says cannot convert to line or arc thus I cannot finish my design because I cannot get the dimensions on the page. All advice appreciated. SW2007
Did you try to insert model items? You could always add points in the drawing view too. Make them coincident to the points on the elipse and then dimension from point to point to show the overall length and width of the elipse.
Steven Danasko, CSWP
SolidWorks 2007 - SP2.2
UG NX3
Pro/Engineer Wildfire 2.0
I do not know what you mean by inserting the model as that is what I am trying to dimension within the drawing space but that is a good idea about putting points on the parts of the elipse That should work. I will have a go and let you know Many thanks
Insert model items - this will insert dimensions, cosmetic treads, datums, annotations, etc. into a drawing view.
From the drop down menu "Insert", select Model items - you can then select a "source". There are several different options that you can select, and this may help.
Steven Danasko, CSWP
SolidWorks 2007 - SP2.2
UG NX3
Pro/Engineer Wildfire 2.0
There is no single dimension you can put on an ellipse to define its size. Ellipse size is 2-dimensional. Typically, ellipse size is defined by major diameter and minor diameter. Sometimes, eccentricity is used.
In sketches, SW ellipse entities already have points at their major and minor diameters. In a drawing, an elliptical edge does not have these points. However, if you use "Convert Entities" in the drawing to create a sketch curve of the ellipse in the drawing view, you will have points to dimension.
Honesty may be the best policy, but insanity is a better defense.
Thanks for the tip. I used to dimension an ellipse by temporarly turning on the sketch in the drawing which allowed me to pick the quadrants to dimension the major and minor axis. You way is less clicks.
I am having the same problem and what I did was just sketched an ellipse in the drawing. I don't like to do this in a drawing but sometimes it is a necessary evil.
Along these same lines I am having an argument with my boss on how to fully define the ellipse. If you dimension the major and minor axis is it fully defined? Do you need to specify that it is an ellipse on the drawing?
Major and minor diameter fully define the size of an ellipse. Location can be made to ellipse center or tangents. If ellipse is not "square" to the drawing, you may need to show the angle of the major or minor diameter centerline.
If your boss still wants to argue, have him take it up with Euclid or Newton.
The usefulness of the Auxiliary view would depend upon how it is to be machined/manufactured. The material at the edges of the ellipse may need to be normal to the profile.
Some machines recognise elliptical geometry, others need lots of dimensioned points to be able to "connect-the-dots".
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Honesty may be the best policy, but insanity is a better defense.
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