How Much Can You Tolerate? - Using Tolerances Inside Autodesk Inventor Models.

“Tolerate, change, or be grateful.”
~Anonymous

The ability to create and evaluate tolerances has been around for several releases in Autodesk Inventor.  I actually can't remember when it was a "new" feature.

But it doesn't seem to get much notice.  I'm not sure how many out there know it even exists.

So I took a moment to put something together to show the steps to setup, and use, tolerances.

Before getting started, let me introduce you to the parts that are going to serve as our samples.

I've created a sample lever and shaft.  Similar to what might be seen on a carburetor butterfly valve, although it's really just a sample.

The sample for this post

With the stage set, it's time to face the next question, where to start?

The first way of adding tolerances to an Inventor model is similar to what you might do on a good, old fashioned, title block.  That step is to add tolerances per the number of decimal places as a title block.

Tolerancing in this fashion is found from Tools>Document Settings, on the Default Tolerance tab.  Here different tolerances can be set for a different number of decimal places.

Locating the Tolerance Values for a part.

For this sample component,I'm going to set tolerances as follows.
.
.00     = . +/-.015 inches
.000   =   +/- .005 inches
.0000 =   +/- .0005 inches

Adding standard tolerances.  It's almost like a title block!

Once these are set they will display on the modeling screen.  Different tolerances can be applied to different modeling dimensions by editing, and right clicking on a dimension and choosing Dimension Properties. .  Here the tolerances can be set by changing the dimension to match whatever the desired model tolerances are.

Right click and choose Dimension Properties

Setting a tolerance via a standard tolerance.

However, there are plenty of other cases where special tolerances must be used, such as deviation, limits of various types, or any other tolerance that may not fit the default tolerances for the model.

To "fine tune" tolerances by adding a special tolerance in a sketch first edit the sketch.  Once the sketch is being edited, use the same as we used before.  This time, use choose the type of dimension to be placed with the flyout.

Choosing a dimension type

If you're trying to add tolerances to dimensions for a hole feature, edit the feature, and left click on the arrow next to the dimension you wish to add a tolerance to.

Setting the tolerance on a hole feature.

Now a tolerance can be added just like the sketch dimensions.

The tolerance is set with a deviation tolerance

But what if you want to change the tolerance on something like an Extrusion or Revolution?  If you take the time to check, neither of the previous tools will work.  So how do you add a tolerance for those features?

Don't worry, there's still a way.  On the Manage tab, edit your Parameters.  All the dimensions for the part are shown here, and by choosing the arrow next to the dimension (similar to what we did in the hole feature), the tolerances for any of the dimensions driving the part can be changed.

User Parameters to set tolerance

So now tolerances have been added to the desired dimensions.... So what?  How can the limits of the tolerance be evaluated?

In each of the tolerance dialog boxes, and in the Parameters screen, there are four icons that change the size of the feature, based on the tolerance you choose.  The available options are upper, lower, median, and nominal.

For example, let's evaluate the pin and it's mating hole at it's maximum material conditions (smallest hole diameter and largest pin diameter).

To do this, edit each part in turn, and add the desired tolerances.  I'm going to use deviation tolerances, since I always found these to be the hardest ones to evaluate by hand.

After changing the tolerances in each feature, I'll set each feature to evaluate at the maximum material condition.  For the shaft, this is the upper side of the tolerance, for the hole, the minimum.

Choosing the smallest possible tolerance dimension

Choosing the maximum tolernace size for the shaft.

With these values set, I can return to the assembly level, switch to the inspect tab, and run an interference check.

Even though the parts are in tolerance, there's an interference

In this example, there is an interference that lays well within the acceptable tolerance I've created.

So what does that mean?  There's work to do?  The nominal sizes and tolernances will have to be adjusted so they don't interfere under any size that still lies within the range of the tolerances.

And what does this mean for everyone else?  

Take a look at tolerances in Inventor, and see how it can help you.  It's always cheaper to find the mistakes in the computer, than in the shop!

And finally, a couple of  "Pro Tips".

There's a couple of small tricks I learned as I worked with tolerances, so I'm going to add them here.

1. Rename parameters.  When setting tolerances, especially when using the Parameters screen. It makes it easier to know which dimensions and parameters you want to change!  There's a tip on how to do that in "Tips for Short Attention Spans".

Using named parameters

 2. Use the Document Settings "Modeling Dimension Display" to set the default dimensions for your model.  Any dimension placed will take this number of decimal places, and by default, the tolerance associated to it.

Choosing the tolerances

4, Change the precision of an individual dimension.  One option when editing a dimension's property, there's an option to change its display value.  This can make sure that you can see an accurate value for the dimension.

Changing the precision of an individual dimension

5. Use the dimension display options to your advantage.  Changing the dimension display will change how your dimensions show on the screen, and can make sure you get an accurate result.

Add caption

For example.  Using "Show Precise Value" will show exactly what the dimension's current value is.

An underline under the dimension indicates that the dimension is currently being evaluated at a value other than its nominal value.  In other words, it's set to be evaluated under one of it's tolerance values (maximum, minimum, median).

6. Explore the tools!  Many of the different tools and dialog boxes share common tools and dialog boxes.  Use that to your advantage.  You can access Document Settings from Dimension Properties for example.  You can change the Evaluated Size of a dimension from the individual dimension properties, or from  the Parameters screen, or from the Dimension Properties dialog box.

And if you've got a sketch active, you can change the dimension display from the dialog box!  Take a look!

Changing Dimension Display.

Whew!  This post did end up being a lot longer than I had planned.  But I hope you find the info valuable!

Five Quick Tips for Autodesk Inventor Assemblies

Avengers Assemble!
Marvel Comics

Over the course of the last few months, I've created tips of things that I thought others might find useful.  So far, I've created one for sketching, and part features  Now for the next step in the series, five Autodesk Inventor Assembly tips.

I've stated it in my previous tips, but I'll say it again.  These aren't in an order, of preference, just the order I jotted them down in.  Take the ones you like, and use them in any way you like!

1) Granted, this a bit of a repeat from part modeling, but this tip works well assemblies as well.  And that's the "Select Other" tool.

When assembling components, Inventor allows us to rotate components while adding constraints, I use this all the time, especially with my 3DConnexion device.

However, there are plenty of times that I don't want to rotate the parts when adding constraints, and this is where select other can come in real handy.

2) Other times when adding constraints, I need to place a lot of constraints quickly.  This is particularly true of insert constraints.

Inventor has another way of placing constraints that has been around as long as I can remember, but seems to have been lost over time.

That method is the Alt+Drag method.

In short, select the geometry to be constrained while pressing the "Alt" key, and the appropriate constraint can be selected.  Drag the constraint to the mating part, release the Alt key, and the constraint is placed.  All done without touching the constraint icon.

The act of using Alt+Drag

It's not a big time saver for a few constraints, but when placing several, it starts to add up.

There's more information from my earlier blog post here! 

3) Another tip I picked up over the last few years came from users who worked with a lot of sheet metal.  It's a creative use of the Flush constraint.

When selecting a small edge to be mated to another, it can be difficult to get the desired face.  Mate, being as flexible as it is, can start picking edges and points near the edge of the face.  It makes it tricky to get what you want.

One option is to use the Select Other tool, just like I mentioned in Step 1, but there's another approach that I think might help everyone out.

That approach is the Flush constraint only see faces.  Starting with that as a constraint, will easily pick the face.  All that is left to do is switch it to Mate once the face is selected.

This can be a huge time, and patience!

Here's a tip on using a flush constraint to pick a narrow face

4) This one has happened to me more times than I want to admit. I've started out with two parts that I swear are totally identical.  I have those components constrained into place, and everything is just about set....

Then I realize that there's one feature that makes one instance of the part different from the other...

Classic.  Two parts I thought were the same, and I realize they're not when they're already placed.

Fortunately, there's a tool called Save and Replace Component.  It's located on the Productivity flyout, and it's perfect for exactly this situation.

Locating the Save and Replace Component tool.

Save and Replace Component creates a brand new copy of the existing part, and swaps the new part for the old.

The bonus?  No constraints are lost, and you can quickly make the changes that make the part unique!

The result with very little inconvenience! 

5) Finishing up the assembly tips, one last one is a tip for a set of features introduced in Inventor 2014, but might have gotten lost in the forest that's created by so many new features.

It's not available in 2013 or earlier, so sorry for those on the older versions.

All of these sets are from the same group, so I'm combining them in together as a "super tip".

First, is to drag a part using the Free Move command.

In previous releases, this just moved the part away from the assembly, regardless of constraints.  But now it shows "bands" between the moved part, and the components it's constrained to.  It's a visual map to how the constraints are behaving. This also includes glyphs showing you what type of constraints are in use.  Right clicking on the glyphs lets you edit, modify, modify, and delete constraints.

Using the Free Move command to show constraint relationships

The other tools are on the Relationships tab.  They're Show constraints, Show Sick constraints, and Hide All constraints.  The name says it all.

Show constraints displays the constraint glyphs for a component that you select.

Showing Constraint Glyphs

Show Sick constraints will show constraints that have conflicts with other constraints.\

Showing Sick Constraints

Hide All constraints turns off all the glyphs.

Hiding All Constraints

I know I've grown to like these tools as I've used them, but it can be easy to overlook them.

So if you've been upgrading and forgot about these tools, take a look!

And I know.  There isn't a video for this one.  Things have kept me rolling where I haven't quite been able to create videos.  I'm hoping that things might just wind down enough where I hope to create one soon!

****Edit 31-December-2014****

At long last, I had the time to create a video to accompany this post!  Take a look!  I hope you find it helpful!

And Happy 2015!