Hydraulic Manifold Drawings
Hydraulic Manifold Drawings
(OP)
I'm working on a hydraulic manifold drawing. I created the model using Hole Wizard for the fluid path features, and Library Features for my various cavities. In total I have the following:
24x Hole Wizard paths
4x SAE-6 ports
3x VC08-2 cavities
2x VC10-2 cavities
1x VC08-4 cavities
When I try to import Model Dims, I am not getting any useful dimensions. From those that deal with this sort of thing every day, what's the best approach to linking my Hole Wizard info in the model to my drawing? I'd like to have associative dims. How have you done this?
24x Hole Wizard paths
4x SAE-6 ports
3x VC08-2 cavities
2x VC10-2 cavities
1x VC08-4 cavities
When I try to import Model Dims, I am not getting any useful dimensions. From those that deal with this sort of thing every day, what's the best approach to linking my Hole Wizard info in the model to my drawing? I'd like to have associative dims. How have you done this?
MadMango
"Probable impossibilities are to be preferred to improbable possibilities."
Have you read FAQ731-376 to make the best use of Eng-Tips Forums?






RE: Hydraulic Manifold Drawings
If you would like a copy of the ports we have, #4 - #20 o-ring, 18 Sun, and 6 HydraForce, e-mail me at danzco@thurston.com
RE: Hydraulic Manifold Drawings
I'm really looking for a way to get my Hole Wizard information for drill size and depth to be associative in my drawing. When I Insert Model Dims, all I get is XY position.
MadMango
"Probable impossibilities are to be preferred to improbable possibilities."
Have you read FAQ731-376 to make the best use of Eng-Tips Forums?
RE: Hydraulic Manifold Drawings
We then create an annotation manually calling out the port, for example....
Ø.201 X 2.18 DP.
1/4-20UNC-3B X .75 DP.
or more generally..
TAP DRILL X 2.18 DP.
1/4-20UNC-3B X .75 DP.
The trick we use to make them associative is when creating the annotation, with the annotion box open, click on the imported dimension on the drawing. Looking at the completed annotation, you will see something like:
<MOD-DIAM>"Hole Dia.@Sketch20@Section-3@Drawing View2" X "Hole Depth@Sketch20@1195.190-1@Drawing View1" DP.
You will have to manually bring the diameter sign into the note as well as after clicking on the hole diameter type-in the <space>X<space> before clicking on the hole depth dimension.
Then simply hide the linked dimensions on your drawing.
If you don't understand what I'm trying to explain, I can send a simple example. Also the 1195.190-1 above is a reference to the part file name/instance.
Remember...
"If you don't use your head,
your going to have to use your feet."