Workflow Questions

[tyson_hernberg]

Hi, I'm new to Inventor and was wondering how complex machines/creations are created in Inventor? Do I make each piece individually and then add it to an assembly or create it all in one project? What does a professsional workflow look like? I know this is all down to personal preference but I would like some advice to start. Thanks in advance!

[johnsonshiue]

Hi Tyson,

This is a very broad question. Here is the answer provided by ChatGPT on "What is the best approach to design a large assembly in Autodesk Inventor?"

Here is the best approach to design a large assembly in Autodesk Inventor:

1. Plan and organize: Before starting the design, thoroughly plan and organize the assembly structure, components, and their relationships. This will help you avoid mistakes and make the design process more efficient.

2. Divide the assembly into subassemblies: Dividing a large assembly into smaller subassemblies can make the design process more manageable and improve performance.

3. Create components: Start by creating individual components that make up the subassemblies. Ensure that each component is complete and accurate before moving to the next step.

4. Assemble components and subassemblies: Open the Assembly workspace and create a new assembly file. Then, insert the individual components and subassemblies into the assembly file and position them relative to each other.

5. Apply constraints and mates: Use constraints and mates to define the relationships between components and subassemblies and control their movement and orientation. This will ensure that the components move and behave as intended.

6. Optimize the assembly: Use the Assembly Navigator to manage the assembly structure and optimize the mates and constraints. Avoid over-constraining the components and reduce the number of constraints where possible.

7. Use assembly groups and suppress components: Use assembly groups to simplify the assembly structure and suppress components that are not needed in a specific view to improve performance.

8. Analyze and test: Use the Motion Study tool to simulate the assembly's motion and analyze its behavior. This will help you identify any issues or areas that need improvement.

9. Document and update: Document the assembly for future reference and collaboration. Make any necessary adjustments to the components or assembly and update the Bill of Materials (BOM).

It's important to keep performance in mind when designing large assemblies. Use the best practices, tools, and techniques available in Autodesk Inventor to ensure that the design process is efficient and effective.

Courtesy of ChatGPT

Point#8 is confusing. The Motion Study (SWX) should be replaced with Dyanmic Simulation or Drive Constraint.

Many thanks!

[tyson_hernberg]

Thanks so much, this is very helpful.

[A.Acheson]

Most inventor users like to model to how it is in reality breaking large assemblies up into the size and components manageable by the assembly team. What industry are you in? Can you show an example of a typical assembly you would like to make?

You likely would use the bottom up approach, creating small parts adding to sub assemblies and then creating larger assemblies. You can also use a parent part to create solids from which you can use make components button  to create children parts and add them directly to an assembly. They are automatically constrained as you have drawn them in the parent part. 

[IgorMir]

There are many ways to do it. If you surf that very forum for a while - you will see the question was asked and answered on far more than one occasion.
In a nut shell - any assembly in the world can be defined by three parameters: Width, Height and Depth. The aim of your modeling is to create such a robust model that if, at one time or another, there is a need to change any of these parameters - the model updates without any errors. 
To achieve that - I, for one - rely heavily on Muscular modeling workflow. What is it was answered in this forum alone tens and tens of times. Please look it up.

Cheers,

Igor.

[3D4Play]

ChatGPT. Utterly disappointed in that reply.

[tomasz.sztejka]

What @johnsonshiuewrote will work if You design a machine created by somebody else. Only then You know how it looks and what parts it will contain, and only then You can use the bottom-up design work-flow.

If however You need to create the machine by Yourself then this is a completely another story. You can't start from parts because You don't know how do they look, right? You have to start from some boundary conditions, ie. floor plan, and build "sketchy" parts on it. Of course "sketchy" parts will be far, far off from the final parts. So if You will assemble them for testing and later update to be less "sketchy" Your assembly will break with many "unresolved constraints" in the future. Also, please remember, parts do depend on each other - a hole must match the bolt and etc.

In an ideal world change in one part would make dependent parts to be re-computed automatically.

Sadly Inventor is rather bad in that manner. It can be forced to be really helpful, but even a very careful and experienced user must be prepared to expect tragic Inventor failures in designs with complex dependencies. What happens near the dead-line of course.

In summary, if You need to draw or model a complex machine in Inventor - follow  @johnsonshiue excellent suggestions. If however You need to create a machine from the idea to the final product, and You need to be prepared to do handle a change of input data at any stage of design, support user configurable options, and You need to be hell efficient in that... well... Maybe You should also investigate other CAD products on the market?

[IgorMir]

That's exactly how Inventor works. 
There is no need to "forcing" anything on Inventor. But the operator's common sense and some practical thinking is a must.
Cheers,

Igor.

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@tomasz.sztejka wrote:

In an ideal world change in one part would make dependent parts to be re-computed automatically.

Sadly Inventor is rather bad in that manner. It can be forced to be really helpful, but even a very careful and experienced user must be prepared to expect tragic Inventor failures in designs with complex dependencies. What happens near the dead-line of course.

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[tomasz.sztejka]

>(...)That's exactly how Inventor works (...) need to "forcing" anything(...)

By "forcing" I meant: a lot of work is necessary since it breaks with complex adaptivity, and it breaks with complex projections, and it flips dimension because does not support directed (signed) dimensions, and it does not allow to select solution for tangent constraints and... Did I forget something? Maybe it does not allow linking logic parameters? Maybe...

It is a good program, but it is a real struggle when You try to use it to work with complex, nested, fully parametric and continuously changing design. The path which allows one to use without faults it is narrow and full of strange and unexpected traps.

[IgorMir]

Ah Tomasz, who was saying anything about adaptivity? 🙂

The "strange and unexpected traps" are there for those, who are not yet familiar with the software. But eventually those "traps" will be no more.  For those, who are keen to learn, that's it.
 

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@tomasz.sztejka wrote:
>(...)That's exactly how Inventor works (...) need to "forcing" anything(...)

By "forcing" I meant: a lot of work is necessary since it breaks with complex adaptivity, and it breaks with complex projections, and it flips dimension because does not support directed (signed) dimensions, and it does not allow to select solution for tangent constraints and... Did I forget something? Maybe it does not allow linking logic parameters? Maybe...

It is a good program, but it is a real struggle when You try to use it to work with complex, nested, fully parametric and continuously changing design. The path which allows one to use without faults it is narrow and full of strange and unexpected traps.

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[Frederick_Law]

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@tomasz.sztejka wrote:
By "forcing" I meant: a lot of work is necessary since it breaks with complex adaptivity, and it breaks with complex projections, and it flips dimension because does not support directed (signed) dimensions

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Adaptive was turned off long time ago.

Master Skeleton removed "complex projection".  Only project/derive from Master.

Flipping dimension can be fixed with dimensioning from center line.

Conveyor collection with different "config".  They were done long before Model State.

Everything is in the assembly, including nuts and bolts.

Conveyor can be lengthen, shorten and not a single hole/bolt will "flip" to the wrong side.

Some of them were tilted.

Lots of other thing were designed with Master Skeleton:

Robotic welding cell, Milling fixture, Welding fixtures, HVAC platform, Part testing machine, Ultra Sound testing machine.

Console and kiosk sometime just start with the screen, keyboard (before touch screen), printer and payment device.

Start a MS.  Assemble/put those parts where they supposed to be and work on the enclosure.

Fixtures are similar.  MS, assemble part, add locating/clamping points.  Built the structure.  FEA.

[tomasz.sztejka]

Thanks. In my case even projected from master breaks at unexpected places. Sure, skeleton is much more robust, but not fool proof too.

But putting all aside this is the way I wished this discussion to be moved towards, as the @tyson_hernberg asked about a workflow in complex cases. Both Yours, and mine workflow is far, far away from what @johnsonshiuewrote.

Can You elaborate a bit about "(...)Assemble/put those parts where they supposed to be and work on the enclosure(...)"? Do You do design enclosure separately or somehow make it to follow "those parts"? If the second, how do You do it? For me it is either adaptive or derive from assembly-project-create new body-derive that body-make new assembly with all parts and enclosure together as a starting point for next part.

What do You do with Your assembly next? Is that Your primary assembly which will get into a final documentation or just a helper assembly?

[Frederick_Law]

There is a "helper" assembly.

Beside the Master Sketch part file, I'll use another Master Assembly.

I use the MA to "transfer", "convert", "project" sketch/feature from purchased or referenced parts to Master Sketch.

Adaptive is not required because those parts won't change.

This way I keep all down stream parts referencing Master Sketch only.

I'll put Master Sketch in assemblies so I can constrain parts to it also.

Most parts should mate/fix/ground to origin but some parts got reused in different location in the assembly.

With a "full detailed" Master, you should be able to make parts without entering any dimension.

All part should constrain to origin or with 0 distance constrain to Master.

Removing or changing any part should not affect other parts.

Only derive the sketches you need in the part.  This will reduce a change in MS causing everything need update.

Name and organize sketches.

Don't do "chain" project (sketch 1 to sketch 2 to sketch 3) in MA.  Project from the source only.

A Chain force dependent on everything before it, instead of only the one it need.

It completely defeat the purpose of using Master Sketch: remove cross dependent between parts.

[johnsonshiue]

Hi Tomasz,

I did not write the paragraph. It came from ChatGPT and I agree with what it said and what you said.

Many thanks!

[tomasz.sztejka]

Thanks for an explanation. Valuable information. Especially the idea of moving back from assembly to master sketch. But don't You need here any adaptivity?

Now, for better understanding what I am saying I would like to share more details about my work-flow.

I usually do design some, very simple compared to Yours, tooling (holders, shapers, molds, testing equipment, manipulators and etc.), but I need to do them in stages. First I design "rough" sketchy parts, test them against the purpose (ie. PCB which I need to be manipulated by tooling) and etc. At this stage they should "adapt" to adjustable goals, but are not fully detailed yet. I do also arrange them on the assembly. Sure, I could add some master sketch and do it by defining locations on the "Master Sketch Part". It would work probably in a most robust way. I am just used to regular assemblies and regular constraints because I can mate surfaces without need to manually compute proper distances in a "Master Sketch".

At this moment I usually needed some "adaptivity" to project resulting distances, shapes and etc to do new parts or more accurate versions of those "rough" sketchy ones. Unfortunately, and as all of You have pointed out, it breaks as hell.... but ONLY if I will modify parts which are taking part in any constraint in that assembly which either directly or indirectly drives the adaptive sketch.

This is the moment when I decide: either derive new parts from the whole assembly or derive each part from its own "rough" sketchy part, place it in the assembly by constraining coordinate system to coordinate system of the original and make it adaptive. I have found that both methods are equally robust. Adaptivity does NOT break if You do not touch parts which drive the adaptive projection.

My next stage is to fine tune "rough" parts to make them "final" or semi final. I usually do it in many steps, since I must match additional futures between them. So Yes, I do have a chain of derived parts, most frequently each level of that chain with own helper assembly.

And a final step which is unavoidably involving deriving parts - machining them, either by CNC or 3D printing. I need to derive parts since each method of machining has own peculiarities. For an example my favorite 3D printing requires me to enlarge all holes a bit to have proper size after print, split parts to have them printed in favorite orientation and from required material and etc.

Usually I don't need may drawings nor final, formal documentation. I suppose if I would need it, I would have to struggle a bit more. I have found that interactive DFW of the final assembly is enough for guys who do assemble the stuff.

Disadvantages? Many files, many updates.

Gladly I can "update all depending on" using one-click macro I wrote which scans all files in projects, builds dependency tree and updates it a right order.

Thanks again for sharing Your method.

[Frederick_Law]

Information flow:

You CANNOT go against the arrow.

Master has to know everything.

Any info from part or assembly going back to Master will create a circular reference.

Change Master, part update, part cause Master to change, Master update part again .....

Master Assembly usually start with Master Sketch with a few sketch, planes to locate/constrain reference part.

Edit MS in MA.  Create plane from reference part.  Project edge from reference part etc.

I have adaptive turned off.  Reference can move by constrain in MA and Projected edge will follow.

MS get more sketches to create new parts.

Sometime I assembly part back in MA to check.  Becareful NEVER project part to Master Sketch.