Automatically unite bodies created by "instance geometry"

[Sillen]

Hi,

I have a complex body with many sketches, extrusions and subtractions. This body will occur in different instances depending on what the customer wants. Is there any way to automatically unite the bodies created by instance geometry?

I have tried using instance feature, which would unite the instances in the same step, but 391 features caused an internal memory access error.

A boolean expression would be nice but the NX boolean expression seems to be something else.

Running NX6


Thanks in advance,
Sillen

 

[jerry1423]

What version of NX are you running?

What do you mean by " . . . but the NX boolean expression seems to be something else. " ?

 

[Sillen]

Hi Jerry,

I'm running 6.0.5.3 and will keep doing that for probably 8 months.

All I've found in the Help about boolean expressions is:

"Creates an expression to support alternate logical states using Boolean values of “true” or “false.”

Use this data type to represent an opposing condition, such as the suppression status for the Suppress by Expression and Component Suppression commands.
"


I don't fully understand what it means but my feeling is that I cannot use it for instanced bodies, hopefully I'm wrong.

 

[jerry1423]

"true" means the boolean is turned "on" . . . in other words a body that needs to be united to another body is just that.
"false" means the boolean is turned "off" . . . those two bodies would then not be united

 

[Sillen]

Sorry for this stupid questions but is there a possibility to add a group of bodies or an instance of bodies to a boolean expression and if so how are they added?

Thanks in advance.

 

[jerry1423]

What you do is first create the boolean of the instances.
Then you can supress that boolean by an expression:

edit (pull-down) > feature >Supress by expression > select the boolean in the model tree > OK

Then go to your expression list and the last "p" expression will be a "1" (true) - now change that to a "0" and the boolean will be turned off.

There are a few options in the "Suppress by Expression" menu that you can experiment with, such as the "expression option" pull-down - if you have questions with that then be sure to post them.

 

[JohnRBaker]

As I hope everyone has discovered by now that the Expression type 'Boolean' has NOTHING whatsoever to do with the modeling operation known as a 'Boolean' operation, such as Unite/Subtract/Intersect.

The Expression type 'Boolean' is a logic construct making it easier to set-up states where the user is expected to edit some Expression value which then causes something to happen. In the past, prior to String Expressions the most common scheme was to use a numerical values of '1' and '0' equating to 'ON' and 'OFF'. Later when String Expressions were introduced some people started to use things like 'Yes' and 'No', or 'On' and 'Off'. However that still depended on people setting things up right and there was no way to force the user to actually properly spell the keyword correct and there was no standard so we introduced the concept of a 'Boolean' expression which can have only one of two values, 'True' or 'False'.

Note that for the next version of NX, we have also added a new Attribute type 'Boolean', which has been preprogrammed to be either 'True' or 'False' and since it will now also be easier to pass Attribute values to an Expression (or back again), this can provide an even slicker scheme for setting up a user-initiated action by simply changing the 'Boolean' status of an Attribute.

I know this response was not a direct reply to the original question, but it was obvious that there was some confusion between 'Boolean' Operations in Modeling and the Expression type 'Boolean' and thought that we needed to clear this up once and for all.

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.com/museum/

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

 

[jerry1423]

oh

 

[Sillen]

Ok thanks for that input. Is there however a way to unite an instance geometry feature (the solids created out of the instance)like unite group or simply put a unite all bodies in part.

Would appreciate if there are any ideas out there.

 

[JohnRBaker]

Rather then using the Instance Geometry function try using...

Insert -> Synchronous Modeling -> Reuse -> Pattern Face...

...and after adding your the united feature that you wish to replicate, use this function to make instances of the faces of the resulting feature. This should give you waht you're looking for.

Note that in the next version of NX we have implemented a new 'Pattern Feature' function which will allow you to select the feature itself and if the original feature was united to the main body, all of the 'instances' will be united as well.

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.com/museum/

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

 

[Sillen]

Thanks for the tip John. Unfortunately I have left the office and won't be back until Tuesday but I'm very eager too try it out.

Seems like there's a lot of improvements in the next release, really looking forward to try it out.

 

[Toost]

In NX6:
If the maximum number of instances are 391,:
Create a "instance geometry" array where total instances = 391 and then unite the target to the 391 tools.
Now you should be able to reduce the number of instances and the unite still be ok.
The problem is that the unite keeps track of the "id numbers" of the bodies that was united and a new #392 instance is therefore unknown to the unite operation.

In NX7.5 the Booleans have "selection intent" such that one can select the instances using "Feature bodies" and therefore the number of instances can both increase and decrease.