Obliquing dimensions in Isometric view

[FishNut]

Greetings drawing experts,


In our sales drawings to customers we need to show top, front, right, and isometric views of our product (an assembly). My problem is with dimensioning the isometric view. We need to show some overall dimensions. For the life of me we cannot get the dimensions in a drawing iso view to show up isometric, like they do in the model when you are modeling it. The dimensions we need to show up isometricare dimesions created in the drawing, not existing dimension in the assembly, so this is not a show and erase issue. The assembly is parametric with dozens of parts swapping out, so we would like to create the dimension at drawing time, because its different components each time. Solid works and solid edge do this no problem, but in pro we can't do it. Or do we just not know how?? We are using wildfire2 m240.

 

[magneplanar]

Fishnut,

perhaps you need to set this in your drawing .dtl/config.pro:

allow_3d_dimensions yes

or

allow_3d_dims (possibly set in your drawing itself)

that should allow you to have dimensions on your isometric view. If you have issues then search for the proper use of these options...

or try here:

http://www.d-digest.com/procluesdigest/v2i8/proclues4.html

cheers,

M

 

[mjcole_ptc]

The Option is
allow_3d_dimensions no, yes
Determines if dimensions are shown in isometric views.

This is set by the drawing detail_config file which you can edit from
File > Properties > Drawing Options



Michael


Edited by: mjcole_ptc

 

[FishNut]

Thanks Magneplanar, Youhad my hopes boostedfor a while anyway. But those settings seem to apply to show/erase dimensions. I talking about a isometric view of a cube, for example.You go to insert a dimension ( a created dimension) for the height of the cube, then a placement point. If you drag you mouse far enough behind the cube, the dimension extends into the Y plane for that model, but if you drag the mouse to the right the dim flips into the X plane.I find it very hard to believe that this is not possible.

 

[vlad1979]

I don't think it's possible what you are looking for at least in wf2. What I do is create dimensions in assembly and show those, edit / setup / dimension if I need dimensions for the overall assembly.


Or show thedimensions from parts in the assy drawing with show/erase if I need a dimension from a specific part.

 

[mjcole_ptc]

Fishnut
If you select two points or vertices and not edges of the cube you will get options for placement type Horiz, Vert, parrallel, diagonal etc. You will have to select from a menu manager dialog that pops up. Lazy programing for wildfire.

Stop living in the past PTC.

Michael

 

[vlad1979]

Fishnut
If you select two points or vertices and not edges of the cube you will get options for placement type Horiz, Vert, parrallel, diagonal etc. You will have to select from a menu manager dialog that pops up. Lazy programing for wildfire.

Stop living in the past PTC.

Michael

Yeah but that's not the true dimension. You will need to fake it ( @o ) to show the real dimension.

 

[FishNut]

I ended up using something just like vlad1979 had suggested, insert, model dataum, annotation feature. It puts in a dimension just like vlads method, except vlads menu picks probably make more sense, so I'll probably usehis method.


Either way I suppose its a way to get it done, but it is not very fast. We use this mostly for isometric details in the drawing. I certainly apreciate everyone's help and input in this matter.

 

[mjcole_ptc]

Yeah I totally agree with vlad's menu pics If you want to create 8 dims why do you have to repick annotation type parallel plane and all that crap again. They should add a reapeat last annotation type option in the new annotation UI.

Vlad's method is extremely fast but the new method using Datum Annotation would let you select it in your model Tree and Show in View which isn't possible with the Reference ad## dims that show at the top of the model tree when the Annotations Filter is checked on.

Michael