How do you get vertical dimensions in a drawing view?

[ScottHeiden]

Is it possible in a dimetric drawing view to make a dimension line showing the Y-dimension distance between two lines?

I'm trying to show how high above the bottom of a table leg the table top needs to be installed. The edge of the table top extends past the table leg, so I have no edges to choose that are vertically in the same plane.

When I pick the visible edges to create a dimension line (this is a dimetric view, so there isn't much to choose from) I get a dimension measuring the straight-line distance between the two parallel edges (the hypotenuse of the rise/run triangle). Is there a way to make this dimension line show the vertical (rise) distance between the two parallel lines instead?

I called my VAR, and they "helped" me eliminate all of my dimensions and notes in the drawing; does anyone out there know if this measurement can be created in a drawing?

Scott

 

[CorBlimeyLimey]

I think you will need to "cheat" and add a sketch (in the part) with geometry which creates an intersection of the points you need to dimension to.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[ScottHeiden]

Thanks, CBL!

I think I'll just add a note stating how high the desk top needs to be above the floor. I'd like to use dimension lines so it'll be noted the same way as all the other info in the drawing, but not for that much work.

Just got an email from Javelin - they suggest placing two points on the drawing view and dimension between them. Nice try, but you don't get an accurate measurement and (most important) the dimension lines aren't parallel to the other dimensions on the drawing view.

I'm surprised Solidworks doesn't allow you to show only "Delta X,Y, or Z" values for dimensions - those values have to be calculated anyway in order to determine the straight-line distance between the objects.

I'd also like to be able to specify which plane the dimension lines should be parallel to (Top, Front, or Right). It's frustrating to me - I know how to do all this if I was working with Autocad...

Scott

 

[handleman]

Can you attach your dimension to a planar face and an edge rather that both edges?

 

[ScottHeiden]

I don't think you can use a planar face for measuring within a drawing or dimetric view in a drawing. The dimension options for Vertical, Baseline, Ordinate, etc. don't seem to work with this Dimetric drawing.

 

[smcadman]

http://img359.imageshack.us/my.php?image=dimetrictabledimensionhp8.jpg

If image is too small and unreadable, you may have to save it and reopen it using your desktop image viewer.

Flores
SW06 SP4.1

 

[handleman]

What version of SW are you using? I'm on 2006 SP4.1 and I can select planar faces for placing dimensions in an iso, di, tri, any metric view.

 

[smcadman]

I'm using SW06 SP4.1 (look at sig). If you look at the screenshot, you will see that the table top and the legs are on different planes in 2 directions (back and side). That is why they do not show up incorrectly. Not only will the dim be incorrect, but it will not be vertical (parallel to the legs).

If you can dimension it without using construction lines, please let me know because I have had to cheat this way for some time now.

Flores
SW06 SP4.1

 

[fcsuper]

First, make sure you view is True, not Projected. Then see if you still have this issue.

 

[smcadman]

The screenshot above is using "True" for the dimension type. I hope you have more up your sleeve than that because that didn't work. Supposedly that should work though:

SolidWorks specifies Projected type dimensions for standard and custom orthogonal views and True type dimensions for isometric, dimetric, and trimetric views.

Flores
SW06 SP4.1

 

[ScottHeiden]

smcadman;

Thank you for making up the drawing - this kind of help is what's so great about this forum.

I was hoping to have the vertical dimension line run along the same planes as the 18" and 24" dimensions in your drawing.

If I added the line as a sketch in the table assembly as CBL suggested, then picked the top edge of the table and the end point of the line the new dimension lines should run in the same directions as the 18" measurement, right?

In my case putting in the sketch causes more problems for me later on. We make Dimetric and perspective views of our assemblies, and any sketch that's active bleeds right through the assembly (as an aside, E-drawings doesn't have this problem: why can't Solidworks behave the same way as E-drawings?).

If the dimension is really important, I think I'll start adding sketch(es) to my assemblies in order to create these dimensions, then turn off the sketches after I've made my drawing. It's just extra work to do something I think Solidworks should be able to do within the Smart Dimension command.

Scott

Scott

 

[handleman]

Flores, my question about version was to Scott, I wasn't ignoring your sig.

Have you tried selecting a line and a plane? When I do that I get this:

http://img526.imageshack.us/img526/7112/tableys0.jpg

 

[CorBlimeyLimey]

As handleman stated, you can dimension between planar faces (not planes) of non-ortho' views.

1) Activate Hidden Lines Visible for the view to be dimensioned. This is not necessary but helps to know where to click.

2) Click the Dimension icon

3) RMB in an area where the first face exists & use the Select Other option to choose the correct face

4) Repeat 3) for the second face or select an edge or vertex

5) Place the dimension


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[CorBlimeyLimey]

any sketch that's active bleeds right through the assembly

You don't need to have the sketch active in the model assy. You can show it only where needed in the required drawing view.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[TateJ]

http://img208.imageshack.us/my.php?image=dimetrictabledimensionhp8bua4.jpg

I got it to work fine...

Windows XP / Logitech "Premium" Optical mouse
SolidWorks 2006 SP0.0 / SpaceBall 5000
Lava Lamp
www.Tate3d.com​

 

[TateJ]

...updated my profile data.

Windows XP / Logitech "Premium" Optical mouse
SolidWorks 2006 SP4.1 / SpaceBall 5000
Lava Lamp
www.Tate3d.com​

 

[smcadman]

Are ya'll dimensioning a model file or a drawing? I can dimension the top to bottom from a part/assembly model, but I do not have an option to pick planes on a drawing.

This is what's great about helping others; sometimes we learn something new ourselves!


Flores
SW06 SP4.1

 

[TateJ]

drawing...

Windows XP / Logitech "Premium" Optical mouse
SolidWorks 2006 SP4.1 / SpaceBall 5000
Lava Lamp
www.Tate3d.com​

 

[CorBlimeyLimey]

smcadman ... you cannot pick planes in a drawing view, but you can pick planar surfaces per my post above.

In TateJs case, selecting an edge of a leg would have given the correct dimension.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[ScottHeiden]

I'm sorry I haven't been able to respond lately - work has gotten in the way of my Forum time;-) I'll be back this weekend.