Associated depth values for cutouts in a solid block

[BOPdesigner]

I am making a shipping case that has a foam insert with cutouts that match the objects that will be shipped in it. What I want to accomplish is with the drawing view looking normal to the cutouts, specify the depth of the various cutouts using notation similar to what the result would be if you applied the feature parameters of a hole. For simplification, consider the following in NX 6. A 4" cube with a sketch circle extruded into it (a hole but not using the hole tool). Now, what I want to do is in drafting, add the dimension of the Diameter of the hole which works fine, then append the depth of the hole to that by doing something as simple as clicking on the bottom floor of the hole and the top face of the block to define the depth value and have it remain associative, but I don't think I can do that. I have discovered that I can click on the Relationships tab in the Text editor of appended text and link to expressions in the part file that represent the hole depth. The problem is that there are a bunch of them and not all the depths are simple (Start = 0 and End = something nonzero). Some have different start depths and are created from different levels below the top face of my part. Are there other options I might not know about? I also don't really want to populate my feature tree with a bunch of measurement feature expressions to link to. I am seeking a quicker method.

 

[JohnRBaker]

Creating a Measurement and linking to it is going to be your only general approach which will always work.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[hudson888]

If you use holes some of the data can be used as annotations on the drawing. But for other kinds of features such as extrudes, then you may need to take associative measurements and construct relationships to those expressions within your annotations.

You If you can measure the distance between geometry then you can make that measurement associative which saves it as an expression. You need to be in the 3D workspace to do create associative measurements. If you're working in master model concept with the drawing separate from the model then the place to create these measurements is at the drawing level. Then as you add dimensions or notes you can use the relationships tab inside the annotation editor to include a reference to the expression.

This method is rather manual and perhaps not ideally optimised for your purposes but at least it gets a result. From a drafting point of view I would expect that the reason it isn't directly available is that it just isn't a supported standard.

Also you may by default get two decimal places as this kind of text is formatted differently, look too adjusting the format field as you add this text from 0.2 for 2 decimal places to 0.0 for none or 0.1 for one. Once added the note will take the form of <X0.0@p37>, where X is the number of decimal place (here set to none, and p37 is the referenced expression).

Once you become familiar with this method you may choose not to create measurements but to add relationships to expressions in the model part files using the same method but clicking on link to part. If you can identify the expressions that you used to build the model in the first place then you will have a manual way to create them as part of your dimensions on the drawing.

P.S Always state what version of NX you're using.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[BOPdesigner]

Rats. Anyway I am trying this. Creating measurements in the drafting file (modeling app). Then I go to the master model and change the depth of a feature and when I go back to the drawing the depth value does not update. I have to go to the feature tree and right click and edit parameters on the measurement feature to get it to update. Why did it not update automatically?

 

[phillpd]

I've just noticed a similar issue with Distance Measurements not automatically updating.

You don't say what version you're running, but my problem is with NX6. Tested it in NX7.5 (beta) and it's the same there.

First reaction from GTAC is to use Feature->Playback. Tools->Update for External Change will also correct it. I agree that these options will force the update, but a user may not know that the Distance Measurement is actually wrong. After all, they'd expect an automatic update.

Specialty Engineered Automation (SEA)

http://www.sea4ug.com

a Siemens PLM Solutions Partner

 

[hudson888]

Either in your customer defaults or session wise turn make sure that updates aren't disabled, and also if you use partial loading, expecially if you're loading lightweight geometry then you may have to change to the solid reference set or fully load the components before the update is possible.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum