2D dimension questions

[CALCAD]

How does one dimension a part to an intersection as in the first image below, and how does one dimension to an apex as in the second image? Thanks.

[A1DWG]

CALCAD,

 

I guess you have to do it the old school way - draw some construction lines on a layer that you can turn off for printing and dimension to those.

 

One question, the shapes you have drawn (look like reinforcing steels to me) have you been given exact sizes for them- If so how did you draw the shapes?

[CALCAD]

Thanks A1DWG,

I was able to get the dimensions I needed by following your suggestion. When you create a line, there is a check box in the properties dialog to make the line for construction. Then, after searching for an embarrassingly long time, I found the layer icon and was able to create a new layer, move the construction lines to it and turn it off. I guess I was hoping for a more direct way. I've got a long way to go to be competent in Solidworks.

 

The drawings in my first post came from Intellicad. Just simple geometry drawn as an example, nothing special.

[shift1313]

which version of SW are you using?

[CALCAD]

I just upgraded to 2009 after using 2008 sp4 for a couple of months.

[shift1313]

you should be able to do those dims in SW but i havent personally tried it and i do not have a copy in front of me. Because of the holidays it will probably be a few weeks.

[dbgeek]

Draw the two lines dimension them and use the sketch fillet command.

 

[CALCAD]

dbgeek,

I think you misunderstand the area of my ignorance. Your solution is, I presume, for drawing a sketch when modeling a part. My problem occurs when making a drawing layout from an existing part. There seems to be no convenient way to dimension to an intersection of planes at any angle other than 90 degrees, or to dimension along a plane to the outside tangent point of a arc greater than 90 degrees, i.e., to the apex.

[CALCAD]

In the first image, I started smart dimension and drew the .300 dimension between the picked points. Then I right clicked the dimension and picked the option Align to Edge, then picked the edge I wanted the dimension parallel to. The second image shows the resulting .209 dimension, which is wrong! To verify the error, I then dimensioned the alignment edge and got .248, which is correct.

WTF? Do I have a bug? Did I do something wrong?

[cedar]

to dimension to the tangent of a rad/cir... while dimensioning, hold the SHIFT key and pick the radius.

 

SW has a tool that will sketch an associative sharp corner. see "Virtual Sharp" in help.

[CALCAD]

After playing around a bit, I confirmed that one can get the tangent of a radius for dimensioning with the SHIFT key. And the VIRTUAL SHARP is what I was looking for to get the intersections. Also I discovered that although the HELP file says the CTRL key should be used while picking the lines for a virtual sharp, the SHIFT key works as well. Thanks again, Cedar.

 

For those trying the VIRTUAL SHARP function for the first time : You need to be in SKETCH mode. Hold down the SHIFT key and pick the two lines, then release SHIFT and click on POINT from the SKETCH menu. Then, depending on the setting of the VIRTUAL SHARP display options, you may see a couple of floating extension lines at the intersection or a plus sign or star.