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Hydraulic Manifold Drawings

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MadMango

Mechanical
May 1, 2001
6,992
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?

MadMango
"Probable impossibilities are to be preferred to improbable possibilities."
Have you read faq731-376 to make the best use of Eng-Tips Forums?
 
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To make port cavities for hydraulic manifolds we chose to create our ports as cut revolves. These sketches can be copied and placed on planes and positioned quickly. As to dimensioning the cavities, we found it simpler to specify the tool, just give a few dimensions to check, usually 1 diameter and the locating shoulder depth, then include the drawing of the cavity from the manufacture. Anyone machining these blocks should buy form drills and reamers for the VC cavities, and port tools for the SAE-6. The exception, when we use Sun pilot operated checks in log grapple cylinders and are subjected to pressures over 6,000 psi., we single point turn and thread this cavity to reduce thread tolerance, and seal clearance. This will increase blow out pressure to about 18,000 psi.
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
 
Thanks for the offer, but we already have a library of features that cover the cavities we normally use.

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?
 
You can get the drill diameter's and depths to import in a view 90° from the view where you get the x-y dimension's to import.

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>&quot;Hole Dia.@Sketch20@Section-3@Drawing View2&quot; X &quot;Hole Depth@Sketch20@1195.190-1@Drawing View1&quot; 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...
&quot;If you don't use your head,
your going to have to use your feet.&quot;
 
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