Dimension Attachment to Centerlines et. al.

[cmarinelli]

While we all love the automatic insertion of dimensions from the model into the drawing, has anyone found an automatic way to attach the end of the dimension line to the end a hole's centerline? SW does not seem to do this unless you make a new dimension and select the hole's centerline. I find it annoying to have to manually move the dimension's endpoint to the edge of the centerline and create an offset by eye.

Dimensions also don't attach to a tangent edge. Here's an example: if you extrude a cylinder, then extrude a hole on one face and dimension the hole to the outside of the cylinder. When you make a drawing, the dimension doesn't attach to the tangent edge.

Anybody have an easy way to handle these?

Thanks in advance,
Chris Marinelli
Dynatech Engineering

 

[Standing]

If I understand your question:
While in the drawing after dimensioning between two holes (Right Mouse Click) RMC on the dimension that you inserted between to holes. LMC properties. Now in First arc condition: pick Max and in Second arc condition: pick Max.
Hope this helps.
Bradley

 

[TateJ]

I - for one - do not "love the automatic insertion of dimensions from the model into the drawing".
They never go in cleanly, and I always have to move them around.
Secondly, the dimensions used to create the features are hardly ever the same dimensions I'd want to see if I were making the part.
Thirdly - and finally - I often want to see ordinate dmensions on drawings; not possible with INSERT MODEL ITEMS.
I guess this is just my ID - Inner Drafter - acting out.
I submitted an enhancement request on this already.

To answer your original question:
If you are INSERT MODEL ITEMS-ing you dimensions, how can you then drag the "end of the dimension line" after the fact?
It's my impression that if you could move it, you would change the dimension value.
Maybe Bradley has your answer, looks like he has a bigger dimension-mojo than me.

H_o³
tatej@usfilter.com​

 

[RawheadRex]

No "easy way to handle these" currently exists. These are just a couple of examples of SolidWorks limitations in the area of their drafting module. You're handling it currently the only way that I know how to.

I began "life" as a detailer on the board 15 years ago and have strong attachments to proper drafting practices. I'm convinced that SolidWorks developers are out to give me stomach ulcers, an aneurysm, or induce some other physical malady when it comes to the drafting functionality in the product. Really, I wish that they would dedicate one release to handling the majority of peoples' beefs with the drafting in their product. I've used it since version 97Plus and it has come a ways but they always seem to stop short and skimp on functional improvements in the drafting module (at least where proper drafting standards are concerned).

 

[drawoh]

cmarinelli,

Dimension ends to hole centre lines:

Are you talking about the hole centre marks, applied to the top views of the holes, or hole centre lines, applied to section views of the holes?

Dimensioning to the Tangent Edge of a Hole:

Create a construction line that runs from the hole centre to the edge of the arc. Constrain it, and apply the dimension to the end of the line. If you construct this in your model, the automatic dimensions will not include the line.
This can all be done using points, but I think it is more work, and you have a less attractive drawing.
It would be nice if SolidWorks let you apply these directly, but I am not sure how they would do it.

My Two Cents Worth:

I agree with Tate] about automatic dimensioning. These would work nicely for me if I organized myself to make them work. Unfortunately, I don't want to. I want to organize myself to control the design. When I do the fabrication drawings, I look at them and I ask myself how the dimensions ought to be applied, then I apply them accordingly. The results may have little resemblance to how I applied my constraints to the part model.

 

[cmarinelli]

Bradley: Yes, I how to do it, but in a drawing, when you drag the handle that is at the end of the dimension line, there is no "point" to reattach to. You can drag it past the tangent point, or 4 inches away from the tangent point. Neither is correct drafting practice. You should be able to snap the endpoint of the dimension to the tangent point, and automatically obtain the correct offset of the extension line from the tangent point.

TateJ: Do you re-dimension a model when you make a drawing? You then lose the flexibility and some of the power that SW provides. What are the advantages. By dragging the handle, I mean the green endpoint of the extension line. You can drag it to lengthen or shorten the actual extension line, not change the dimension value.

Rawhead Rex: I know exactly what you mean. I started out as a Jr. Engineer/Draftsman 10 years ago, and I do get anal about the drawings. When I see something that doesn't look right in a drawing, it immediately makes me question everything about the drawing.


Optech: I'm talking about dimensions that come from centerlines AND centermarks. Usually (at least in my field) holes are dimensioned in the 'top' view of the hole, from the centermarks. The Insert|Model Items command puts the extension line of the dimension coming from a hole right at the center of the hole, not from the end of the center mark as is correct drafting practice. It drives me nuts that I have to adjust the extension line length to fit the centermark.

I'm going to send in an enhancement request on this one.

Thanks for all your responses!

 

[DennisD]

You can use ordinate dimensioning in a sketch and therefore get these on your drawing with the auto insertion. This is really only practical for items defined in the flat, but it is available.

- - -DennisD

 

[TateJ]

cmarinelli:
Yes - I do re-dimension the model in my drawings. Even in the simplest of parts, the dimensions never land in the right place - in my opinion. I know I loose a little functionality - I can't edit the drawing dimension and update the model. But I can live with this rather than the randomly placed INSERT MODEL ITEM dimensions.

Dennisd:
I'm going to see what happens when I use ordinate dimensions in a model sketch. I have to admit, I've never tried it. I have tried to use ordinate dimensions on my features - and failed.
But now that I think of it, I haven't tried it with 2003 yet.
I'll let y'all know how it goes...

H_o³
tatej@usfilter.com​

 

[drawoh]

TateJ,

I have used ordinate dimensioning on my models too, but never when actually constructing them. Usually, I have deleted the external constraints, and I need to apply local constraints. Ordinate dimensioning gets the job done fast.

As I apply the ordinate dimensions to my model, I look at my fabrication drawing to verify that I haven't moved anything. In other words, my fabrication drawing exists before the ordinate dimensions are applied to the model. The ordinate dimensions get applied just like whatever it is I applied to my drawing.

JHG