I think it's because you have an equation driving it and it's forcing the value to change to match the equation.
Yes, having the equation is involved in causing this behavior. But...
the equation does not know or care about whether it's being used as a diameter or as a radius. I definitely think this is a repeatable problem (at the least unexpected behavior to a user). Only I don't know enough about the internals of SolidWorks yet, to be able to understand what exactly goes wrong.
You are not just changing the dimension visually. It is a driving dimension and the value is from a formula so if you change it to a diameter dimension the value is still 95.59. To change it to a diameter dimension then you have to take the /2 out of the equation =( "Outer pitch diameter" + 2.5 * "Module" ) / 2. If want to see the diameter then put in a reference dimension.
Ok, @Solid Air
I can live with knowing that the "view" changes also internal interpretation of the value (I would probably do such differently myself, relying e.g. on the name of the dimension whether it's "R..." or "D..."). But let's say it does. There's still something glitchy in the way SolidWorks handles the change.
1. Halo.SLDPRT > Boss Extrude1 > Sketch1 > Edit
I want to change the D1@Sketch1 dimension to be shown as diameter, like the rest of them.
2. Click on the dimension
3. Right click > Edit equation...
4. Edit the equation to "= ( "Outer pitch diameter" + 2.5 * "Module" )" ("/2" dropped)
( Here, one of the problems is that a user cannot at the same time change the equation, and the viewing mode. Thus, SolidWorks inevitably gives those error dialogs. Just ignore them. = "Continue (Ignore Error)" + Close )
5. OK on the equation manager
(more errors; ignore again)
Now we get a Mickey - like thing on the screen, but that's okay. We know what to do.
6. Edit Sketch1, right click on D1 dimension > Display Options > Display as diameter
NOW, This is where I would expect things to fall back to normal. We've changed the equation and we've changed the "view as". Right?
What I see is:
I'm expecting that to show ... 191.19
7. Exit the sketch > "Exit the sketch and rebuild (feature will show as error)"
Well, the rebuild fixes the thing and there's no error in the features.
Something in this workflow - which I think is pretty common - confuses SW 2018 SP 2.0. Nice part is that it's repeatable and thus likely fixable.
1-Double click on Sketch1 in feature manager tree so sketch dimensions appear in graphics area.
2-Right click on 95.59 dimension, select Display Options, Display as Diameter. You should see your dimension change to 191.19. DO NOT REBUILD MODEL.
3-Double click on dimension to display Modify dialog.
4-Backspace /2 from equation.
5-Click rebuild button and exit dialog.
You will not see what you posted in your screen shot.
When you have several dimensions to change in a sketch, this is the method I recommend to use. Nothing is updated until you rebuild so you do not get the annoying error messages.
I really liked your answer. It helped me understand the behavior better.
Was thinking of clicking it to be "Correct answer" but ... since I think there's something unsolved here that SolidWorks engineers should have a look, it's not fully complete. So my Kudos to you - maybe I find a way to pay back?
It's not "unsolved". Everything is working correctly.
If the dimension was not controlled by an equation, you could switch between diameter and radius without affecting geometry. Because the equation drives, the value is maintained and can not be halved or doubled automatically.
Disconnect the equation from the dimension, change to what you want, then adjust and reconnect equation if you want. Simple.
Your reply would be perfect if you also told how to "disconnect the equation from the dimension".
I'm simply bringing in use cases where I feel the tool is surprising, to newcomers like me. Please be patient with that - I think there's value in collecting this kind of feedback because once a tool becomes too specialized, people "know" to use it "right" (and using it right needs elaborate teaching). SolidWorks is not in this camp, yet. It can be learned by exercising and by wonderful support in these forums.
Just... now I'm searching how to disconnect the equation.
Tried double click on dimension > remove the "=" in front of the equation.
This does the disconnection (no more sigma sign), but also the equation is lost, and needs to be re-entered.
So my recipe would be:
- visit the equation, copy it to clipboard
- remove the "=" as mentioned above
- double click again on the dimension, enter the equation (with edits) from clipboard
I'm sure in 2 years I'll laugh at this and comment on my own thread a superior way to do the same.
Please don't think I'm trying to talk down to you. I just want to help you make sense to something that seems sensible to those who have experience.
Consider the problem you are forcing upon SolidWorks: You are asking SW to automatically change a value which has been explicitly assigned control to an equation by a user. In effect, SW has been told "don't change this, always use the equation". It is doing exactly what it was told to do.
Note that the "Σ" on the dimension indicates that it is controlled by an equation.
There are a number of ways you can decouple the equation. The simplest would be to delete the dimension and make a new one. You can suppress the equation. You can manually assign a value to the equation in the dialog by double-clicking and entering a single value.
1) Delete the equation.
2) Change to diameter dimension
3) Re-add the equation.