Newbie Question about Part properties

[johnEE7T4]

Hello all,

I am trying to understand the best practices for parts, components, assemblies...specifically how can I have a part be recognized into its native features as I import from a step file or even create a part or create a simplified part at the assembly level or create a part or components or derive a part or demote parts. 

I read on youtube that you can use an add in for Part Recognition Feature.

My challenge at the assembly level is I want to build off the grippers (attached) and make a mini fixture that the grippers will integrate with. I think in 2022 there are some advancements where it makes it easier to do this but how were designers doing this beforehand?

I just cant find a way to get the components or parts to have the sketch --> Extrusion, etc parent child relationship so I can modify ...it seems I have to use direct edit or break link with sub assembly base component but I still seem to be unable to see this extrusion or sketch hierarchy. 

I see that there is direct edit and edit solid but this is still not the same. 

I seem to be ridiculously confused on what is the best approach to get the part to be able to have the traditional extrusion and sketch description so I can easily modify. 

All I see are the "+" signs as shown attached. 

Thanks for reading

john

[SBix26]

First: what version of Inventor are you using?

Do you want to modify the grippers, or do you want to design parts to interact with the grippers?  These are two very different tasks.

There is no need to modify the grippers themselves if you are designing fixtures.  You can derive the grippers into a part file as surfaces, and from these surfaces you can design parts to interact with and assemble to the grippers.

But if you want to edit the grippers themselves, you could try the Feature Recognition add-in (may or may not give you useful features); the Direct Edit tools, as you have already mentioned; or model from scratch, using the imported parts as a reference (essentially a manual feature recognition process).

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Sam B
Inventor Pro 2022 | Windows 10 Home 2004
LinkedIn

[johnEE7T4]

Sam,

I appreciate your support and taking the time and respond and your patience. 

I am using 2021. I have seen that 2022 has an improvement in this area.

I want to design apart that would interact with the grippers. 

I struggle to do this at the assembly level and the upper and lower jaws are sub assemblies of  a larger assembly. 

I am going to try to derive the grippers into a part file as surfaces.

Fingers crossed! 

I know Inventor is truly about assembly at the top level and not building components or parts off of it. 

There must be an easier way. I have had mixed success with the Feature recognition tool but that is the exact idea I was looking for.

[SBix26]

Building parts off of a derived imported part is something that is easy to do in Inventor.

I'm still not clear why you need to recognize features for the grippers if you're not actually altering them?

In any case, if you're still having difficulty understanding how to work with them, feel free (if you can) to post the gripper models here and give some ideal of what you're hoping to accomplish.  Naturally, I'm not going to do all the work for you (and I'm sure that's not what you're asking), but maybe I can demonstrate something that will get you going.

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Sam B
Inventor Pro 2022 | Windows 10 Home 2004
LinkedIn

[johnEE7T4]

Absolutely!,

My intent is to add the knowledge to my toolbox. 

I am reading that derived parts can not be edited or cut but only extruded?  Maybe its from an older release. 

I appreciate the input/direction . and will begin to work with the derive feature and report back 

[Frederick_Law]

You cannot get sketch from import parts.  All import are "dumb".

You can recreate the sketches.

[SBix26 · Accepted solution]

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@johnEE7T4 wrote:

I am reading that derived parts can not be edited or cut but only extruded?  Maybe its from an older release. 

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That doesn't match anything that I know about Inventor derived parts (in 19 years of using it), so it's either a poor translation or some other miscommunication.

To use one or both of your grippers to design a mating part, start a new part file as you ordinarily do.  Click the Derive tool, which will open a dialog box to choose the file you wish to derive in.  After selecting your gripper, the Derive Part dialog opens, allowing you to select what you want to derive (sketches, work features, solid and surface bodies, parameters, etc.); you don't have anything besides a solid body or two in your gripper, and that's probably pre-selected for you; at the top, you have a choice of how the solid bodies get brought into the file-- as a merged solid, as separate solids, as a merged solid with faces remaining separate, or as surfaces.  The latter is what you would use for this job.  Surface bodies have no mass, and are transparent by default, so they won't mess with your model properties.

Now you can construct a mating part or parts by projecting important parts of the gripper into new sketches, using faces as terminations for extrusions, etc, etc.

Does that help?

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Sam B
Inventor Pro 2022 | Windows 10 Home 2004
LinkedIn

[johnsonshiue]

Hi! I believe you need Model States in 2022. It allows one ipt file to have multiple geometric definitions. In your case, you can create two model states capturing the difference. You don't need to derive it. Before 2022, you do have to derive it to create another shape.

Many thanks!

[johnEE7T4]

Yeah. I guess I just have to become accustomed to this type of thinking. 

I dont know what drives the programming in the background but was hoping there was a way to import or modify a part to have the native Inventor properties. 

[johnEE7T4]

I am going to try those exact steps tomorrow. thank you 

I did have it mixed up on what I stated like you said ..it was not derive but the construction of parts at the top level 

https://forums.autodesk.com/t5/inventor-forum/not-able-to-extrude-the-sketch-in-assembly-environment...

[johnEE7T4]

Thanks for this clarification sir. 

I see the defense of how the kernel for Inventor was built upon and why the top assembly level is as such where you can not just easily continue to use the traditional planes and build at that level because you can one add to an assembly with top level components.

I need to take a step back and work with the derive function and recognize its effectiveness in building around the grippers so I can design my fixture within the grippers. 

[johnsonshiue]

Hi John,

Do you mind elaborating the exact request a bit more clearly? I am sorry I don't think I understand your latest reply. Please share an example. Forum experts can help take a look and provide further guidance. It is possible there is a better workflow.

Many thanks!

[johnEE7T4]

The upper and lower jaws are actually part of an assembly. Do I first create a simplified part or I can derive form an assembly?

Thanks!

[johnEE7T4]

 I just wanted to add that I brought it in as an assembly and these were my options. I do not see surface. I just see composite. (Please see the snagit attached) Thanks 

[johnEE7T4]

Hello Sir,

I am doing a very poor job explaining because I do not have command of the terminology in explaining how I am trying to design this.

I will try to post up my design or a basic part of it when complete. Its nothing proprietary ..just a phd gripper that I am trying to build a fixture off of. 

Thanks again for the support.  This is unarguably the best source for quick competent but not condescending direction on the net by far. 

[SBix26]

A simplified part is a derived assembly, so it's essentially the same thing. As you've discovered, you can derive an assembly, and Composite is the choice you want-- that will be a collection of surfaces.

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Sam B
Inventor Pro 2022 | Windows 10 Home 2004
LinkedIn

[johnsonshiue · Accepted solution]

Hi John,

I think I know what you are after. You want to be able to create geometry regardless of component structure. Inventor was designed to model traditional assembly modeling, meaning components have clear definition and structured. Geometry is mostly bounded within a part.

I think Fusion 360 will work better for you. You can define the geometry without having to designate it as components. You can focus on shape definition before worrying about component structure.

Do I understand your requirements clearly?

Many thanks!

[johnEE7T4]

Hello all,

Thanks for the clarifications and steering me to the correct path.

I got the model to work via the derived approach and I just need to understand the way of the "traditional assembly modeling" design philosophy on how Inventor works.

This is by far the most powerful source for Inventor in the world. 

The community members are not condescending, are extremely competent and helpful and the support is very quick.  

[mcgyvr]

@johnEE7T4  I read this whole thread and I don't think your intent or issues were communicated well enough and I think you got answers that didn't apply and steered you in the wrong direction.

Lets break down your original questions..

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@johnEE7T4 wrote:

I am trying to understand the best practices for parts, components, assemblies...specifically how can I have a part be recognized into its native features as I import from a step file

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"native features" aren't stored or translated in STEP files. That data is lost upon converting to a "dumb solid" like a STEP file. You can use any of these techniques to further modify that geometry.

1. Feature Recognition Addin https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=9172877436288348979
2. Adding new native features to modify the existing geometry.
3. Direct Editing techniques.https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2022/ENU/Inve...

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@johnEE7T4 wrote:

 or even create a part 

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Besides just starting a new part file (File.. New and pick a standard part template and just start creating sketches/features) I think you want to create a new part BUT have access to the geometry of your existing gripper.. If so you can create a part in the context of an assembly to allow you to use/project geometry from other parts in that assembly. (in the assembly just press the "Create" button in the "Component" section of the Assemble tab.)

https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2021/ENU/Inve...

It seems like you may not need to modify your existing imported gripper parts but just want to create additional parts around that. 

Personally I start by creating a single part file and getting some geometry established then create an assembly and place that part into it.. Then I just keep creating more parts and adding those parts to my assembly and modifying any of the parts as needed based on measured dimensions of other parts,etc... that just works easier for me and I'm just used to it.. I rarely if ever edit or create parts in the context of the assembly as its just not how I started doing it.

Others do everything right from an assembly creating new parts as they go all in that one assembly window. 

It sounds like this should be your workflow..

1. Open your imported part and save it. This will give you an Inventor ipt file that you can use. It won't have editable features unless you also run the feature recognition tool but as stated above there are ways to modify that specific part.
2. Create a new assembly and place your new gripper ipt file into that.
3. Create a new component in the context of that assembly and start modeling any new parts you want to also be part of this assembly. 
4. Repeat Step 3 for each and every new part you want in your assembly model.

Hope that helped a bit more. 

If not it really may be time for you to more clearly define exactly what you are trying to do in small increments to avoid it just being too much to tackle at one time. Break it into pieces..