Generative Design

The second half of this year has been pretty busy for me.  One area that I have invested a lot of my time has been learning Generative Design.  I still remember being at Autodesk University when Autodesk first started talking about this technology.  They had a bulkhead from an Airbus plane.  They talked about how much weight they were able to remove from just that one subassembly.  I knew then that this would be the future of design.

It has been a few years, but I have really had my first opportunity to really get into Fusion 360's Generative Design process and learn how to perform the design studies.  It really is a powerful technology and even though the studies are done in Fusion 360, I have sought ways to bring this ability to Inventor.  Through this learning and investigation, I have come to discover that Fusion 360's Generative Design process can be used on almost any file.  If you are using Fusion Team, you can use the Desktop Connector to sync your local files to the cloud.  Then use Fusion 360's Any CAD ability to place the Inventor model in a new Fusion 360 design.  If you can't leverage Any CAD, then you can always export and import an STP file.

Regardless of how you get your design into Fusion 360, either by designing right in Fusion 360, using Any CAD, or importing an STP file, you will need to do some sort of setup.  Generative Design has two key geometry definitions, Preserve Geometry and Obstacle Geometry.  Preserve Geometry is a body, or bodies, that need to be part of the final design.  They usually represent key connection points.  Obstacle Geometry is a body, or bodies, that need to be avoided in the final design.  Both of these can be component bodies or bodies modeled specifically for the design study.  You do have the option of creating a Starting Shape, which is a body that represents the shape you want to start with.  This is not a requirement and I don't often define a Starting Shape.

Preserve Geometry

 

Obstacle Geometry

The Connector Obstacle command does a great job of allowing you to define assembly hardware as obstacles.  You can pick a hole and define a bolt, with or without a nut, shown as cylinders.  You also can define a tool clearance, shown as another cylinder, which will ensure you have access to properly assemble your components.

Connector Obstacle

After you have all of the Preserves and Obstacles defined, you can begin defining your Load Cases.  Load Cases are Structural Loads and Constraints that represent different scenarios that your design is going to face.  You can apply static forces, pressure, moments, bearing loads, and remote forces, which were added in November of 2020.

Next comes defining your Objectives and Limits, this is where you can define the objectives for the study.  You have a few choices as to what types of outcomes you are looking for.  The most common is the Minimize Mass with a minimum Safety Factor.

One of the best parts of the Generative Design workflow in Fusion 360 is that it is manufacturing aware, meaning, that we can identify potential manufacturing methods and the study will take those into consideration when generating the outcomes.  We have choices of Unrestricted, meaning it will just generate the best shape possible, Additive, 2 1/2-Axis Milling, 3-Axis Milling, 5-Axis Milling, 2-Axis Cutting, and Die Casting.  Each will have its own specific parameters.  There is also the ability to enable cost estimation for the outcomes.  This enables you to enter the number of pieces you need to make and Fusion will use the aPriori database to also estimate manufacturing cost.

The last criteria you will have to define is the materials.  You can define the potential materials that are being considered for the component.  You can set materials for all manufacturing methods, or you set specific materials for specific manufacturing methods.

After all the setup, you can then Preview the outcome.  This is a good idea because it can help you see if you forgot to include a preserve or obstacle, which has happened to me once or twice.  

Then it is time to run the study.  The study will be done in the cloud.  When Autodesk first introduced this workflow, it cost 25 Cloud Credits to calculate the outcomes, however, they have since removed that cost.  Now the only cost associated with running the Generative Design Study is just a cost of 100 Cloud Credits per outcome that you generate an actual design file from.  The time it takes to fully calculate all the outcomes is a combination of how many manufacturing methods and materials you have chosen.  For me, it usually takes a couple of hours, but the actual time will vary.

As the study outcomes are being generated, you will be able to start looking at the results.  There are different display modes for the results and the left-hand side of the dialog gives you the ability to filter the outcomes of a variety of factors.  One of the newer enhancements is that you will receive recommendations as to which ones are seen as the best possible outcomes.

I could go on and on about filtering and sorting individual results, but the goal would be to export an outcome to a design file.  That would be better as another blog post soon, so this will all for now.  Hopefully, you will be able to leverage this workflow, regardless of which tool you use as your primary design tool.  

If you would like to see more, please watch my recent webinar on how to perform a Generative Design Study on an Inventor model.

Inventor Feature Properties

 Last week, I had a support call that the solution ended up being a familiar, yet relatively unused function of Inventor.  I had already been using Inventor for years before I found it and  I am not sure how many users even know about it.  I am talking about Conditional Suppression of the Feature Properties.  

Inventor Feature Properties users access to several different properties of a given feature in the browser.  It will allow a user to change the name of the feature, create some conditional suppression, enable or disable certain Adaptive elements, and change the appearance of the feature.

In this case, I want to focus on the conditional suppression options.  These allow a user to create conditional suppression of a feature based on the value of a parameter.  You might say, I can already do that with iLogic.  This is true, however, iLogic requires a certain level of comfort with writing VB.net code.  Inventor Feature Properties don't require any code and offer an alternative to users that are intimidated by iLogic.

The premise is really simple, you can access the dialog by right-clicking on a feature in the browser.

Once in the dialog, it is just a matter of defining the conditions of the suppression.  

The user can enable If then build and expression related to a parameter.  Your choices for parameters will be limited to any parameters of that feature and any parameter with a meaningful name.  Then it is a matter of picking the typical equation types, such as equals, does not equal, greater than, greater than or equal, less than, or less than or equal.  When it comes to the value to test for, it can be a static value or another parameter values.

Here is a simple demo video of how this can work.

This is a pretty simple command, but it is capable of quite a lot.  It is just a matter of identifying driving relationships.  At my job, we get a lot of requests from our customers to help them add automation to their designs.  We will typically lean on iLogic for that automation, but before we do, we consider if something like the Feature Properties can help us accomplish the given task before we jump to iLogic.  So think of the Feature Properties the next time you need to create some conditional suppression.

Bringing a Little It's A CAD World to Autodesk University

 Every year Autodesk conducts Autodesk University or AU at locations all over the world.  It is the opportunity for Autodesk software users, industry experts, and Autodesk employees to gather together to share knowledge.  This year, in light of COVID-19, Autodesk has elected to host one virtual global event, which will be held November 17th to 20th.  Whether you have attended AU multiple times, or never attended, this is a great opportunity to grow your skills and knowledge.

You can still register for AU.

https://www.autodesk.com/autodesk-university/conference/overview

I have spoken at AU Las Vegas on a few occasions and since this year is being conducted virtually, I figured I would submit a few class proposals.  Two of those proposals have been accepted.  My class presentations will be pre-recorded next week, then I will be hosting a live Q & A for each of my two classes during the week of AU. 

The classes I will be teaching at AU are Vault & Inventor Properties:  Working Together for Better Data Management and The Essential Skills for Sheet Metal Modeling in Fusion 360.

Vault & Inventor Properties:  Working Together for Better Data Management is an in-depth look at the Inventor iProperties and Vault Property systems.  I will be discussing the differences between the two systems.  Then I will show how to create properties and mappings between the two systems to create a seamless experience for end-users.

The Essential Skills for Sheet Metal Modeling in Fusion 360 will cover the basic skills necessary for creating sheet metal models in Fusion 360.  I see a lot of posts in the Fusion 360 Facebook User Group from people that are looking for resources on how to get started in different areas of Fusion 360.  I felt that this class would be the perfect opportunity to create a resource for sheet metal modeling.  I will discuss the purpose of the Sheet Metal Rules and how the Flange command can be used to create three different types of geometry.

You can find these two classes and many more in the AU Session Schedule.

https://www.autodesk.com/autodesk-university/conference/schedule

If you do have the opportunity to attend, I hope you check out my classes and attend the live Q and A session for one, or both, of the classes.  It would be a great way to connect to those of you that have been reading this blog over the last few years.

Hope to talk to you then.

Inserting Parameter Values into Drawing Text

The last parameter workflow that I wanted to share is how to insert a model parameter into a drawing note.  It is a feature I rarely use, but I don't do production work full-time.  The process is pretty simple but will link the value from the model to the drawing note text.  You will be at your most productive when you can create these types of relationships which cause Inventor to do the bulk of your time-consuming tasks.

To illustrate this, I thought about scenarios where drawings have notes about unmarked fillet radii.  This is where filleted edges are not dimensioned but the user will place a note that reads, "All unmarked fillets to be 1/16 in."  To make that note more intelligent, I could create a user parameter named FilletRadius, then use that parameter when creating the required fillets.  When I add the note on the drawing, I could insert the FilletRadius parameter's value into my note, instead of typing that value out.  Which would save me from having to edit the note if the FilletRadius value changes.

So the first step would be to create the necessary Model or User parameter.  For my example, I am going to create one called FilletRadius.

Then I need to create the Fillet features that use that value as the radius value.

The last step would be in the drawing file.  You start a Text Annotation as usual and type and static text that you need in the note.  For my example, I would type, "Unmarked radii have a radius of."  To get the User Parameter into the annotation, I configure the drop-down menus above the text pane.  Selecting the file, User or Model parameter, the required parameter, and the precision.  After those selections are correct, you can click on Insert Parameter, which will insert the specified value into the note text.  Then you can finish the note off with any other static text.

Here is a video demonstration of how to insert the parameter.

That is all there is to it.  Again, this creates a dynamic link between the model parameter and the text note.  This will eliminate having to update the model value and the note text if the unmarked fillet radii change.  The scenarios of where this can be useful are numerous.  Hopefully, you can use this technique to build similar relationships between model parameters and text notes.

Automation Through Linked Inventor Parameters

Building automation into Inventor models is one of the biggest requests that I hear in my job.  Customers have a few projects that they have built and they want to find a way to leverage that and build new projects faster.  In most cases, the designs have variations in them that make them unique.  When I review these customer models, looking for ways to add automation to them, I first look for ways to utilize basic Inventor functionality before considering custom programing.  One of the easiest ways to get automation into a design or project is to link parameters.  

A model's parameters can be linked to either another model or an Excel file.  Once the parameters are linked, changing the values in one location will cause the linked parameter in all the other locations to update.  In most cases, the local update icon will light up in the other files, letting you know that Inventor sees new values and wants to update the models to reflect the new values.  The process of creating the link is pretty simple but can be very powerful and save time for the user and eliminate mistakes.

To link parameters to an Inventor file or Excel file, you will first need to open the Parameter dialog box and click the "Link" button.  

Inventor will then display the Open dialog, where the user can filter based on the file type they are looking for.  

If an Inventor model is picked, a dialog box will be displayed asking which parameters you would like to link.  

If the selected parameters are not marked for Export, Inventor will ask if it is okay to mark it for export.

Once that is done, Inventor will bring all the parameters into the parameter list.  

If an Excel file is picked, the user can also pick the Start Cell for where Inventor should start reading parameter values. 

Then Inventor will add the parameters to the list.

Here is a video demonstrating the process of linking parameters between Inventor files.

Here is a video demonstrating the process of linking parameters to an Excel file.

Having done this multiple times, I have a few tips that will save you from errors and make the process more manageable.  First of all, even though you can link parameters between models, Inventor will complain about a cyclical reference if you link parameters between an assembly and one of its parts.

If you prefer to control parameters by linking between Inventor files, you could create a separate file that holds all the parameters and then link the models to that file, as a shared resource. 

If you want to link parameters to an Excel file, you have to put all the values on the first tab in the file.  I have seen customers create multiple tabs for different calculations, then push those values to the main tab.  Also, when you link the parameters to an Excel file, you will be asked for a start cell.  Inventor will then start reading that column for parameter names and use the next cell to the right as the value.  If it sees a blank row, it will stop reading values.  By using different Start Cells and blank rows, you will have better control of which parameter values get pulled into which files.  One limitation of this is that you will not be to link one part file to a specific Excel file more than once. 

Lastly, I advise you to keep the parameter names of each file unique.  If you link in a parameter named "Length" and you already have a parameter named "Length" in your file, Inventor will change the name of the linked parameter to "Length_1."  I haven't seen this cause an error or issue, but it might cause confusion.

So that is all there is to it.  Using the ability to link parameters to other models or Excel files should give you an easy way to add some automation to your new or existing project.

  

Inserting Parameters into iProperties

A common challenge Inventor's users face is the need to put model dimension values into iProperties.  For example length, width, and thickness values into the description.  Many users resort to manually entering these values.  This usually results in errors because they forgot to update a value when the model changes.  However, manually entering these values is not necessary.  It is possible to link your description or any standard or custom iProperty to a parameter value.

The first step in this process is to understand the meaning behind the Export column in the parameter dialog.

The Export column has two roles.  One is it will allow the parameter value to be derived into another part during a Derive operation.  The other role turns this value into a Custom iProperty.  I use the Export column for this purpose more frequently than for Derive operations.

Simply checking that box isn't all there is though.  Since parameters are typically entered as decimals, it may be necessary to format the value in the custom iProperty.  Also, you need to understand the formula for getting the iProperty value into another iProperty, i. e. the Description.  To illustrate how to do this, I am going to use a wall panel similar to one I would have made back in my days in the RV industry.  I have made the part as a rectangle that I extruded, then added a few cutouts.  To make creating the formula easier, I like to give my parameters meaningful names, so I name them Length, Width, and THK.  I can then check the Export column for those three parameters.

Then I want to make sure that Custom iProperty associated with these parameters are formatted the way I want.  Right-clicking in the Equation Cell for an Exported parameter will show the command to format the iProperty.  

In this dialog, I have options such as decimal or factional, precision, and unit string.  The Apply to existing comparable parameters options will also format other exported parameters the same way.  This can save a lot of time since you won't have to format each parameter individually.

Now, opening the iProperty dialog and jumping to the Custom tab, I will see the three custom iPropertiers that were created by exporting the parameters.

The formula to insert these into another iProperty isn't that difficult.  It is just a matter of starting the value with an equal symbol, to signify that you are going to be creating a formula.  Then anytime you want to insert a parameter, you enclose its name in <   > symbols.  So in my case, my Description will be =<THK> Panel, <Width> x <Length>.

This formula method will work in an iProperty and will allow you to pull from any iProperty.  Once a formula is entered, the iProperty will display the result of the formula.  If you need to edit the formula, clicking the function symbol next to the iProperty will display the formula, so you can edit it if necessary.

Here is a video demonstrating how to accomplish this.

Taking Parameters to the Next Level

Accessing a model's parameters in Inventor gives a user access to many functions.  You probably have changed values directly in the Parameter dialog.  Perhaps you have even given the parameters descriptive names or created equations between values.  However, there are several functions that are available that are often overlooked. 

Did you know that you can have iProperties pull parameter values?  Did you know that you can link parameters to Excel files or other Inventor models?  You can even pull parameters into text notes in an Inventor drawing.  Leveraging these functions can simplify your daily workload, so I wanted to share some of these often-overlooked parameter functions.  So in the coming weeks, I will be sharing blog posts and videos on how to incorporate these into normal workflows.  First up, will be how to pull parameter values into iProperties.  Come back next week and check that out.