Linking parametric dimensions

[SGEngineer]

I have two dimensions, one describing the hole diameter (with tolerances) and the other describing it's depth (with tolerances). How do I display them in the drawing?

 

[ctopher]

Here is one way:
(dia sym).XXX-.XXX
(depth sym).XXX-.XXX

If for example there are two of them:
2X (dia sym).XXX-.XXX
(depth sym).XXX-.XXX

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[SGEngineer]

In this way the dimensions will not be updated / driven by the model updates.

In addition, I would like to make my bilateral tolerances in a top bottom display. Can this be done?

 

[ctopher]

Dim it, then select properties of dim and change to bilateral. The depth dim may have to do manual.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[SGEngineer]

Do you mean typing in the values for the depth?
How about the tolerances? I can't do another set of bilateral tolerances for the depth.

 

[BiPolarMoment]

You can make the dimensions driving if you import them from the feature into the drawing: Insert -> Model Items -> Select the Feature/drawing view you want to dimension and the dimensions governing that feature should automatically import. If you just want driven dimensions that will update with model changes you can use auto dimension the same as you would in any sketch.

For the tolerances if you select the dimension in the drawing a toolbar will open on the left and there are several options concerning how to display/configure them. If you select Bilateral it will display the tolerances to the right of the dimension with top/bottom as min/max e.g.:
-0.12
XX.XX +0.06

Hope this answers your question.

 

[SGEngineer]

Well, I want 2 driven dimensions displayed in an annotation that shows the diameter w/tol and depth w/tol.

I know that insert model items will work but it shows two dimensions completely.

In another scenario, I have a rectangular cutout with a depth callout but I can't display the dimensions without manually keying in the values.

 

[BiPolarMoment]

Re: Depth

Er, why can't you do another set of bilateral tolerances? You should at least be able to select the sillhouette of the hole for a depth dimension then tolerance it in the same manner you did for the diameter. If you mean that you want the depth displayed in a view that is normal to the hole axis then you would have to just type it as a note.

 

[BiPolarMoment]

Solidworks allows you (rarely) to drag dimensions (shift+drag I believe) from one view to another. So, for example, you could dimension something that is difficult to select in the view and move it. However, I do not think it will let you drag a dimension to a view that is normal to the dimensioned item.

What I would do in if it is imperative to have it driven is dimension from an alternate view (assuming there is one) and drag it near your other dimension, turn off the extension lines (properties->dimension display) and draw your own leader if necessary.

 

[ctopher]

I have turned in enhancement request's several times to allow auto tol for both dia and depth dim in same dim. I don't know if it has changed for v2006.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[SGEngineer]

Apparently it doesn't allow it. The only way I thought of is to create a note and linking it to a created dimension. Then delete the source. However this does not work for the tolerances as it's taking values from <dim> in the source.

I have been working with UG and Pro/E in the past and they both allowed me to create driven notes / dimensions parametrically from the models. Perhaps Solidworks should come out with something.

 

[rporter]

If I understand correctly what you are looking for try this.
Make 2 custom properties one for the dia. the other for the depth. Highlight the box for the value then click on the dim that pertaines to it. Now insert a note add the dia. symble then a link to the custom property. Now do the same for the depth. I have used this at diffrent times mostly on radius dim.

 

[SGEngineer]

I managed to do it another way by adding notes and putting in the link to the model, for instance... keying in "Hole Depth@Sketch4@@Default@TBD Isolator.SLDPRT"

It reflects the dimensions in the drawing but not the tolerances. Still working a way around.

 

[CorBlimeyLimey]

You don't need to key-in the dimension ... simply double-clicking on it will embed it in the note.


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