How to control design features in assembly (similar to work with solids in Inventor)

[pvn]

Hey fellow CREO users,

please share you experience in the way how you control design of the assemblies.

In Inventor I used to creating the part which I'd call multibody and it would be the basic control file for my assembly. I would control the overall dimensions and common features, attachments, etc. in this file and then derive solids into the part adding other design details.

Let's say I have a number of brackets attached to the structure with a attachment points pattern. I need to play around with the dimensions of brackets depending on the attachment points locations. So I would like to look at one part with attachment points and modify another part depending on the attachment locations and surrounding structure.

What is the best practice to do that?

I would like the sketches of these parts to be linked, so if I were to change a hole location in one part it would automatically change it in the other part. Is this something that can be achieved with Creo?

Thank you very much for your help! 

[dschenken]

Look into skeletons.

http://support.ptc.com/help/creo/creo_pma/usascii/#page/assembly%2Fasm%2Fasm_three_sub%2FAbout_Skeleton_Models_in_Top-Down_Design.html%23

You can also create references from one part to another in the context of an assembly, but I would recommend against that if there isn't a lot of thought put into managing them as a group.

There is no identical work path.

[pvn]

Thank you for suggesting skeletons. Haven't heared about this yet.

When working with parts through an assembly, how stable is it? Would my constrains fall through if parts (features) I was referencing will change? That was the main issue in Inventor. Lack of stability when you revise part based on a feature of another part. This is why working with multibodies (solids) was so helpful. 

[StephenW]

I have never had any issues when working with parts inside of an assembly. I do most of my design on parts within an assembly.

[HamsterNL]

Besides the skeletons that @dschenken mentions, you could also look into Publish Geometry & Copy Geometry.

https://support.ptc.com/help/creo_hc/creo30_pma_hc/usascii/index.html#page/assembly%2Fasm%2Fasm_three_sub%2FAbout_Copy_and_Publish_Geom_Feat.html

(Please remove the Google Analytics parameters at the end of the URL, ea everything after the .HTML)

[pvn]

What do you guys usually do? Let's say for a simple example where I need to control geometry of several parts depending on the attachment points between them and surrounding structure?

It's pretty easy to do with my Inventor set of skills, but challenging with this new Creo tool with no experienced live users 🙂

[MartinHanak]

Hi,

please attach picture of design you want to create in  Creo.

[pvn]

Hi @MartinHanak here is an example of the area I am working at the moment. I need to project the hole pattern onto three doublers and adjust geometry of the parts around surrounding structure.

[MartinHanak]

Hi,

I attached simple model using assembly cuts shown on part level. Files were created in Creo Parametric 2.0 M240.

[StephenW]

You can use references to the assembly when you are working on a part within an assembly. I typically do this.

When I finalize my design though, I remove all references of the assembly from the part so my part is stand-alone.

You may or may not want to remove the references, it all depends on your design goals.

Skeletons and publish geometry are features within Creo to help you manage external references effectively.

[pvn]

@StephenW what happens when some of the references you used change? Does Creo picks up the changes and adjusts features accordingly or so you get an error?

[StephenW]

It depends on your reference choices and your changes.

If you reference a hole within the assembly and you later delete the hole, the part that has the reference will have a failed reference that you will need to correct. It will not be "unstable", it will just show a failure and you will be need to specify a new reference at your convenience.

If you change the location of the hole (and regenerate the assembly) your hole in your referencing part will change in accordance.

[HamsterNL]

Talking about references...(I am being slightly off-topic here)

Make yourself familiar with Intent Edges. This video explains/shows the power of Intent Edges:

https://learningexchange.ptc.com/tutorial/14/using-intent-edges-for-rounds

[dgschaefer]

Skeleton models with publish and copy geom features are very robust and enable rapid iteration of design changes.  I don't do any development work without them anymore.  They do require the extra cost advanced assembly extension.

Creo gives you robust reference management that will help you keep your assemblies updating properly.  Whenever you select a reference, either in sketcher or in other features, Creo tells you that reference's ID and the feature it belongs to.  By paying close attention to those you can build very robust yet very interconnected assemblies.  There are also tools for replacing one reference with another, either for individual features or globally.

This is under the umbrella of "Top Down Design" and Creo has a very robust suite of tools for this, with skeletons & copy / publish geometry features being one of the core components.