I have a noob question, but I just can't figure it out.
I've created ordinate dimensions using horizontal and vertical ordinate tool in drawing mode. The first click sets zero and I pick a few dimensions to add ordinate dimensions based on that zero. Now, I have added features after the fact and need to add more ordinate dimensions using the existing baseline, but when I click on the tools it wants to make a new zero point.
How do I add new ordinate dimensions to an existing baseline?
And wouldn't you know it, as soon as I submit the question I figure it out for myself.
Use normal ordinate tool to add dimensions, not horizontal and vertical.
Basically, just RMB on the ordinate you want to add to, and select Add to ordinate.
WT
Right click on any of the existing ordinate dims in the group and pick "Add to Ordinate", then pick the geometry you want to dimension.
OK, How do I set "Current Ordinate Group"?
I tried the RMB on any existing ordinate dimension in any group and pick "Add to Ordinate" then selected the geometry I am trying to dimension to. And I get a message to the effect of, the geometry I selected is the wrong direction for current ordinate group.
See the attached screen shot.
I believe I tried every concievable combination of picks etc. but keep getting denied with this warning.
Any other suggestions?
Brad,
In your screenshot, if you RMB on one of the ordinate dims at the top, select "Add to ordinate" and then LMB on the centerline that's highlighted I would think it would work.
In the warning, it says "current ordinate group"
Which makes me believe that some where, some how, the system is locking onto a specific cordinate dimensioning group.
And if I try to dimension to something that is not in the correct alignment "wrong direction" the system throws up this warning block.
Sometimes it does work, and when it does, I cannot determine why it did in that particular attempt and then not another.
Seems kind of random.
So, anyway to determine or set which cordinate dimension group is currently set?
When you first RMB on an entity of the ordinate group to select "Add to ordinate" it should turn blue, but after that I don't know of any way to determine what group is active. It may be simplest to delete that set and re-insert them.
I am starting to believe the problem is with what I am trying to dimension to.
I am trying to dimension the "center of a rib, represented by creating a "centerline" in my drawing view.
It is these created "centerlines" that I am having trouble with.
Maybe these created centerlines are not square with my drawing view. They look like they are perpendicular etc.
I can create the Zero leader off of any one of them, but then I get the "wrong direction" warning if I try to select another one that should be parallel to it.
In my drawing view the ribs are running vertical on the screen. The face of these ribs is angle back in reference to the direction of view.
So in an orthographic projection view they would not be running vertical.
Could this be part of the problem?
So if it is, then what good are these "created" centerlines? Other than they look good...
OK, so while I have been typing this I have been trying other options as I think of them.
I went back into my model, and created some DATUM planes using the sketch that the ribs were created from.
I made these datums do they would be in perfect alignment with my drawing view.
Worked great, I can dimension to them.
I guess this will be my work around for this particular Solidworks limitation.
I'm glad you got it to work. From what you said, it sounds like the line you started from (the zero leader) is not parallel to the other centerline. Have you activated the Smart Dimension tool and then clicked on each line? If they're parallel it will give a linear dimension, and if not you'll get an angle dimension.
You can also use the Measure tool to determine the relationship between geometries of any type so see what the deal is.
Can I "add to ordinate" in a sketch in a part file?
I can easily do this in a sketch in a drawing file.
Please help.
p.s. It's pretty emotional to see an old post from Wayne! What a great guy.
Right-clicking and choosing "Add to Ordinate" works in Part sketches just like it does in Drawing dimensions. If you aren't getting this option you may need to click on the double arrows at the bottom of the drop-down list and choose "Customize", then select it.
Check the solution offered by Kelvin here in case you still have issue https://forum.solidworks.com/message/564695#comment-564695
else try the video solution from this post https://forum.solidworks.com/message/564736#comment-564736
If you are running 2015 or older, in order to add to ordinate in a sketch, you will need to double click on an existing dimension first.
Then, while the edit dimension window is up, RMB on an existing dimension and select "add to ordinate".
In a drawing, just RMB on any ordinate will bring up the same menu.
Apparently they have fixed this in 2016 and newer.
Right click on any of the existing ordinate dims in the group and pick "Add to Ordinate", then pick the geometry you want to dimension.