An interesting thread appeared on the SolidWorks Forum this earlier this month. A SolidWorks user posted a question asking how to flip dimension text from one side of a dimension line to the other, for an ISO Standard drawing. The perceived problem was that a non-orthogonal linear dimension appears backwards to nearby orthogonal linear dimensions. Is this correct per the Standard?
Why would SolidWorks put dimension text on the wrong side of the dimension line? The user noted that if the dimension is placed on an opposite part (or other side view), the dimension text placement appears to be correct.
Actually, according to ISO standard, the 0.82 dimension is correct in both views! This is because the standard requires the dimension text to be in the most upright position. So, although vertically aligned text is required for vertical dimensions, dimension text should never actually be upside-down. This is a case where SolidWorks is following the rules of the standard, but the standard’s rules produce an affect that seems out of place to some users.
But are the alternatives actually better?
What would a flipped dimension look like in this case? What is really the expectation? As it turns out, this answer isn’t so simple, nor is it pretty. There is an ambiguity between two possible methods to flip this dimension.
Although the 0.82 has the same reading direction as the 1.00 dimension, because 0.82 is nearly upside down, it is difficult to read.
This method is easier to read. But it still looks incorrect because it is actually opposed to other nearby dimensions. It also appears to be incorrect because now the dimension line is on top of the dimension text, which is more confusing (especially if you have a crowded drawing).
In general, this is a case where something may not appear correct at first, but once you see the alternatives, it really does make sense. These are the reasons why SolidWorks doesn’t support “flipped dimension text”. However, if you would like to use either of these alternatives, there is a workaround. Perhaps I will cover it in a future article.
What if you still want another solution?
There is one aesthetically pleasing alternative that SolidWorks and certain standards do support.
Highlight (select) the dimension.- In the PropertyManager, select the Offset Text button. The dimension text will now be attached to a leader that points to the center of the dimension line. If this is fine, then you are done.
- For ISO Standard drawings, this may not be acceptable yet. If this is the case, drag the leader so that it lines up with the dimension line, and the text is outside of the extension lines. This requires a little bit of eyeballing, but nothing that is going to give you a headache.
Now for something somewhat different, check out Angles and their relationships for information on different types of angles.