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Creating two configuration in NX10: Base model and premium model

Hi All,

I have a model that needs two configuration. Customer has requested me to create base model which has less features and a premium model which is having features built on base model. Now I would like to link the premium model to the base model,i;e premium model should get updated when the base model updates.

For examaple:

Base model has features : Body-extrudes-hole-fillets

Premium model has features: Base model(Body-extrudes-hole-fillets)-switch cut-outs(Feature grouped)-added bosses(feature grouped)

Can I use part family for this??. If YES how..

Any suggestions would be appreciated.

Thanks, 

Devaraj

7 REPLIES

Re: Creating two configuration in NX10: Base model and premium model

Legend
Legend

This would just be a simple Assembly.

Create the Base Model.

Add Base Model as a component to an Assembly File.

Wave Geometry Link the Base component to create an assosiative linked body in Assembly File.

Continue adding Features to Linked Body.

Re: Creating two configuration in NX10: Base model and premium model

Hi  

Yeah, that is an alternative option I have. But I want to have single part which will have two configuration(similar to solid works configuration).

Thanks,

Devaraj

Re: Creating two configuration in NX10: Base model and premium model

Siemens Phenom Siemens Phenom
Siemens Phenom

@Devraj_Mendon, Once base model is complete, use 'Extract Geometry' command with associative, fix at current timestamp to have extracted body as base model. Create a reference set for this extracted body (Base model). Continue work to produce premium model and create a separate reference set for it also to distinguish at assembly level.

 

Part family can also be used where particular features can be included or excluded to specific or all child parts. But it will depend upon the complexity of the final model and how often you need to create/edit such models.

Re: Creating two configuration in NX10: Base model and premium model

 @GaneshKadole,

Thanks for the suggestions.

Hope it works for part file.

Re: Creating two configuration in NX10: Base model and premium model

@GaneshKadole

Can I get separate drawings if I use reference set?

Can Refernce set able to provide two configuration?

Thanks,

Devaraj


@Devraj_Mendon wrote:

 @GaneshKadole,

Thanks for the suggestions.

Hope it works for part file.


 

Re: Creating two configuration in NX10: Base model and premium model

Siemens Experimenter Siemens Experimenter
Siemens Experimenter
You could also use "Suppress by Expression..." where the features for the premium version are unsuppressed by expression value =1. For expression value = 0 just the base part is displayed.
Command is stored under "Menu --> Edit --> Feature"

regards
Andreas

Re: Creating two configuration in NX10: Base model and premium model

Valued Contributor
Valued Contributor

@Devraj_Mendon

 

Configuration in Solidworks is similar to Reference Sets. To be clear Reference Sets are not used to create configurations. That is what a part family is for. You want definite parts that come from a mother model. This mother model is a normal .prt file and can contain lots of different types of geometry and you can control all of the features with Featur Suppression by Expression which @AS3 has mentioned. This is a very powerful thing, as you can create a 150% single part and connect your suppressions and your geometric definitions to expressions which are linked in your Part Family Table(Excel based). You can also create a drawing for each child in the family. And since all these parts come from the same mother I recommend creating a drawing of the mother with dimensions, notes and so on, and then copying this to the other children. When updating the drawings from the children, some dimensions will be disconnected, because the feature has been suppressed for example. These must be deleted which can be done via a script/journal.

 

Reference Sets in NX are different representations of the model. I use it to create Simple geometry. I actually create my geometry in a way, where I can easily extract the body associatively, move it to another layer, and the keep working on the actual detailed model. The extracted body can then be called upon when loading the assembly for example. Another way you can use Ref Sets is by showing the engineer the motion of something. It doesn't move but you see maybe different degree locations in the sense of a valve. If it has a long arm and could collide with something, then you want to show that to the user in form of a 3/4 of a pie, that is been extruded in the model. I know this all sound pretty weird and complex, but it is very useful, because you then do not have to create sub assemblies with arrangements and such. In the sense of a valve, the knob is mostly independent and will not be connected through constraints to something else, to make it move. So in that case you can "describe" it's movement in the form of a turned profile. In terms iof the simple reference set, I can use that for other workflows. Let's say I want to simplify my product. Marketing and sales do not need the guts of the part, just the outside profile more or leass. These comprises of few or many parts, depending on what kind of product it is. If I had an engineering team, I would, among others, make a simple reference set in every single part. For choice assemblies I would also create a reference set with the same name and bring those particular compnents into it, so that I only "see" the outside stuff. If I think a bit further, I could also automate this and run a STEP export on the displayed bodies and then customer, marketing and sales are happy and do not have to carry a bunch of heavy STEP files :-). Maybe you want to support your simulation guys. Well you could also create a Ref Set called Simulation and when your simulation guys load the assembly or part with that particular reference set active, then they will only get the bodies they need for simulating. I put some pictures of an example part on here.

 

In conclusion ref sets are for different states(bending steps of sheetmetal) or displays of the geometry. Yshould not use this for configurations. If you follow the steps @GaneshKadole said with the extracted body and you create 20 configurations, then you will have a pretty long feature tree, which not a lot of people like and most people do not name their features anyway, so no one knows which is the front or the back. At the end of the day, I think creating your model using feature suppression by expression is a super nice route. You control everything through suppressions. That is the most stable. Expressions don't look for edges, faces or other objects, they are just there and they do not know time as compared to features in the tree. Take a look at the pictures, and if you have questions, you can personally ping me. I have created some pretty cool part and assembly families that work like a charm and even have multiple reference sets, so I can simulate or look at it in a simple form. It is possible.

Cheers

Philip

 

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