Tooling From a Solid

I have been using 3D modeling software for so long that I often find myself looking at an object and thinking about how I would model it or how I manufacture it.  Perhaps I am just crazy, or maybe you are just like me.  I found myself doing this on Sunday when I was looking at a church pew.  It had routed edges and a routed pattern on the end.  In this instance, I was thinking about the CNC tool path around the end.

I started thinking about the shape of the tool and how to model the tool.  After some time, I realized that if I modeled the tool, I could also leverage that using Inventor 2020's new Solid Sweep function.  This happens to be something I have seen demonstrated, but I haven't tried it myself. 

I had sometime on Monday morning, so I figured I would try out this workflow.  It worked pretty great, I ran into a few hiccups, but I was able to get around them pretty quickly.  Since it worked out so nicely, I figured it would make a great blog post.  For my trial model, I decided to create a cabinet door, similar to the ones I used to model when I worked for Fleetwood Folding Trailers.

It didn't take long to model up a door and two tools, one for the center detail and one for the edge.  I also wanted to verify how flexible this model would be, so I gave most of the model values meaningful names. 

At this point, I want to note that my tool models were pretty simplified, they were revolved profiles of the shape I needed to cut.  At one point, I did experiment with adding more details to the bit models, for example, adding the cutting edge.  I found doing this did cause my feature to not turn out exactly right.  So I reverted back to the simplified versions, which in reality is still perfectly fine in this workflow and makes the process easier on you.

Here are images of the bits I modeled up.

So the first step in the process of creating a sweep from a solid is to either model the solid or derive it into the current model.  Thinking of how this workflow would be the most useful to other users, I was envisioning having a folder, or catalog, of router bit models, that could be derived into the required models.  So that is why I chose to model the bits separately and derive them into the model of the door.  Deriving the bit model into the door model is straight forward, the only thing to make sure to do is to bring the bit model in as a new solid.

After the bit is derived into the door model, it is important to locate the bit at the beginning of a path line segment.  If you don't, the sweep will not calculate correctly.  See the example below.

To locate the tool body at the right location, you can use the Move Body command, from the Modify pane of the 3D Model tab.  At that point, you can enter X, Y, and Z offset values to get the bit to the proper location.  In the image below, you can see that I have some parameter values driving these locations.  This will make the model easier to edit because those values are driven by the initial sketch in the model.

Once the bit body is in the proper location, you can create a sweep using the bit body as the cutting object.  You will have to enable Solid Sweep when creating the sweep feature.

I did have one odd issue arise when working with one of the sweeps.  When the inner detail was a cutting operation, the model would disappear.  It was like the body was disabled or invisible.  However, I discovered that I could have the sweep create a new solid body.  Then I could use the Combine command to subtract the new solid from the solid body that represented the door.

Here is the finished model of the door, after the two sweeps.

If you would like to see this workflow in action, please watch the video demonstration below.




Now that the model is done and I have IPT files for simplified versions of the router bits, I wanted to see if Inventor CAM would allow me to create milling tools out of those IPTs.  So I entered the CAM workspace and created a Setup for the CNC program.  One of the most important parts of creating the Setup is identifying the stock.  In this workflow, I am envisioning that the panel was already cut from a piece of wood and we just need to create the tool paths to route the edges and the center detail.  So the stock in this case will be the blank panel.  The default option for stock definition is to enter offset values for how much stock is on each side of the model.  In my example, I will set those to all 0s.

At this point, we will need to create the milling operations and create the tools.  It is possible to import the tool while defining the operation, so you don't necessarily need to add the tools to the Tool Library first.  For me, I just added them while defining the operation.  Both of these tool paths will be 2D Contours.  So while defining the first 2D Contour, I went to select the tool, which opens the Tool Library dialog.  I thought it would be best to create a new library to hold my tools, so they didn't get confused with the default tools in the default libraries. 

Once the library is created, you create a new tool in that library.

This will open the New Tool Definition dialog.  In the General tab, you can enter the Tool Number, Description, and several other identification properties.  The Cutter tab is where the IPT files can be imported as the cutter geometry.  For you to be able to import an IPT as the cutter geometry, you will have to set the Type to Form Mill, then the Import File option will become available.  The software will automatically find the bottom of the model and identify vital dimensions form the imported geometry.

From this point, the tool can be selected as the tool for the 2D Contour operation.  However, the rest of the tool path definition is identical to the workflow for creating any other tool path, so I don't want to go into those details here.

If you want to see the complete workflow from importing the tools and the 2D Contour operation definitions, you can watch this video demonstration.


As I explored this workflow, I will say I learned a lot about the new Solid Sweep and defining my own tools.  Hopefully, you will find this information useful and can apply it to make your daily tasks easier.

Inventor: From STEP file to Parametric Model

I have been using Inventor for over 13 years now.  In the early days, when you would import a STEP file, you were mostly stuck with the geometry of the model.  You could edit the model by adding features, but something like moving a hole was not a simple process.

Several years ago, Autodesk added Direct Editing to Inventor, which gave users the ability to edit STEP files, and other imported models.  Direct Editing has given users the ability to move faces, change the diameter of holes, scale the model, rotate features, and delete faces.  An added benefit is that any entered values for these changes become parameters.  So if we use these tools just right, we can take an imported model and make it parametric.

I have explained how to do this in classes for years, so I decided I should write a blog post about it.  Before I make a video or write a post,  I will typically test out the workflow to make sure I don't have any issues.  While testing this workflow, I was slightly surprised by an issue.  I discovered that if the entered parameter values don't change the model, compared to the original imported model, the Direct Edit feature will error.  For example, if the original STEP model is two inches long, and I edit the Direct Edit parameter so the model is two inches long, I will get a model error.  Once I discovered why I was getting the error, I realized that I could just suppress the Direct Edit feature when the parameter changed the model back to the original size.

There are two ways to suppress a feature depending on a parameter value, iLogic and Feature Properties.  I have done plenty of blogs and videos showing how to work with iLogic, so I wanted to use Feature Properties in this case.  I also find that most Inventor users either don't know about Feature Properties or they forgot that they exist.

You can access a feature's properties by right-clicking on the feature. 

The Feature Properties dialog box will allow you to suppress the feature, or conditionally suppress the feature, depending on the value of any parameter.

So how can we apply these to make a parametric part from a STEP file?  We can create Direct Edit features that change the size of the model and use feature properties to suppress the Direct Edit feature if the feature is returned to its original size.

In my sample, I can create a Direct Edit feature that adjusts the length of the part.  If I use the "Measure From" option and the face on the opposite end of the part, the entered value will be the length of the part. 

The entered length automatically becomes a parameter.  Parameters are automatically named d0, d1, d2, and so on.  It is up to the user if they want to give the parameter a descriptive name.  I like to do that because it makes editing them easier.  Since I can name a parameter "Length," I don't have to remember which parameter controls the length of the part.  Renaming a parameter is easy.  All you have to do is open the Parameter dialog box and edit the name field for the parameter.  See the image below.

The last step in the process will be to edit the properties of the Direct Edit feature to enable a conditional suppression.  In the sample shown, the Direct Edit feature will be suppressed if the Length parameter is equal to 2 inches.

I do have a few pieces of advice when applying this technique.  First, you can put more than one operation, or change, in every Direct Edit feature.  I would not do this because the suppression will control the entire feature, not individual operations in each feature.  Secondly, I gave the Direct Edit features descriptive names, I find it makes the model easier to work with and easier to identify what the direct edit controls.  Thirdly, every time we use the Feature Properties to conditionally suppress a feature, Inventor creates another parameter for that value as well.  This can make it hard to find the driving parameters in the Parameter dialog.  Creating an iLogic form of the driving parameters can solve this problem.  The image below shows the iLogic Form I created in this example.  If you like this approach there is plenty of help documents that will explain how to create a form. 

If you would like to see a demonstration of this technique, please watch the video below. 

So even though an imported STEP file has no features at all, we can use Direct Edit to change the model.  Then if you apply those tools in a very specific way, we can turn that STEP file into a parametric model.