In the past, I’ve settled on using the phrase “TO V.S.” after dimensions when they attach to virtual sharps. I’ve seen this type of notation used elsewhere. Another abbreviation I’ve come across is TSC, which I assume stands for Theoretical Sharp Corner. I think that might be older terminology.
Personally, I used to prefer the shorter “VS” because it feels like a more commonly understood term. That said, none of this really matters since the standards don’t specify what’s “proper.” For example, ASME Y14.5-2009 uses the term Point Location but doesn’t provide any identification symbols or abbreviations for this concept.
SOLIDWORKS, on the other hand, generously offers a variety of marks to identify virtual sharps. The main problem? These markers are often so small on certain drawing scales or radii that they’re nearly impossible to see without magnification. Another issue is that none of these marks are defined in any standards. And, honestly, a third problem is the hidden nature of the functionality.
You have to know how to create a virtual sharp mark—there’s no dedicated button or icon for it. It’s a short sequence of steps that you’d never guess without guidance. Here’s how it’s done in a drawing:
- Select the two object lines that intersect in space.
- Use the Point sketch tool.
How is anyone supposed to intuitively figure out that you need to use the Point sketch tool for this? Seriously. But hey, at least SOLIDWORKS provides some method. That’s more than can be said for the standards.
I guess my question is: What are others doing to identify dimensions that reference virtual sharps?
Anyway, here’s an updated article about Virtual Sharps.
Hi fcsuper,
Our Australian Draughting Handbook does mention a method of dimensioning to an ‘imaginary’ point; if what you are referring to is a point that is the intersection of two lines projected from two edges joined with a chamfer or fillet, etc.
The method is described thus, “Projection lines referring to imaginary points of intersection should touch or pass through the points and the points should be emphasized with prominent dots, the diameter of which should be not less than twice the thickness if the line they terminate or 1mm whichever is greater.â€
Having said that, I have never used the ‘dot’, preferring instead to rely on the projection lines and if the are too close to see clearly I would always show an enlarged detail view, of the area, to remove any ambiguity.
I will add; I know many machinists that would, if presented with a drawing dimensioned as described, throw the drawing back at the drafty with the comment – “how the hell am I sposed to measure that†😉
We call them Intersection Points and will label the dimension with IP to signify this. We will also use CPR (Center Point Radius) to clarify dimensions for our machinists.
Cheers,
Anna
We mark about the same as Anna for theoretical corners. While I agree that I would not want to be the part checker, if it is what the vendor wants it is what they get.
In my previous post I referred to what our “standards†said about dimension your ‘virtual sharps’ and how I would draught (in 2D). Today I revisited your question using Inventor to see if it had a solution similar to yours, or whether it had anything at all. I have not required this before when using Inventor and having found what I have I would be very careful I applied it, if at all.
Using Inventor, if a triangle is created as a sketch, dimensioned and then fillets (rounds) added to one or all corners; Inventor maintains the dimension to the original point but shows no projection lines back to the point of tangency between the line and the fillet.
If the parametric model dimensions are used as annotation in the drawing a similar outcome si seen; that is, the dimension extension line is just sitting in ‘space’ not clearly indicating what it really represents and it is not easy to attach an additional notation.
However if – when in drawing mode – a dimension is added manually Inventor can be forced to look for the intersection point (using the ‘intersect’ menu option) and when the dimension is placed it has extension lines correctly aligned to the original edges/lines. There is no ‘dot’ at the intersection.
So that part is fine except if I was in the position of having a very small fillet the end result may not be easily/clearly seen if looking at a large object or as a printed document.
My manual solution, creating a detail enlargement of the area fails in Inventor when using Inventor’s ‘Detail View’ command because having created the enlarged view it is not possible to show/attach dimension/projection lines.
I’ve always referred to virtual sharps as an apex.
I put the term in parenthesis i.e. 3.67 (APEX)
Also, I’d never heard of the term “Virtual Sharp” until I started using Solidworks in ’98. I had always known them as “Theoretical Sharps”.
I have always placed a clarification that states “All dimensions to theoretical sharp corners.” either in the notes or as a part of the title block, say with the other standard callouts like “All dimensions are in inches.” “Interpret Geometric Tolerances per ASME Y14.5M.” etc. these are all collected under a “Unless Otherwise Specified:” statement.
In the cases where it may be unclear what I am intending, I use a separate view with a higher scale for the particular area.
In my experience, it is much more common to dimension to sharp corners than not to, but each working environment and industry demand different things.