Assembly Challenge: Mating a Spherical Face with a Circular Edge

Issue:
Your design requires you to constrain a part with a spherical face to another part with a circular edge. But when you went to apply a tangent constraint between the spherical face and the circular edge you realized that Inventor doesn't allow you to select edges for a tangent constraint.

Solution:
Although you can't apply a tangent constraint in this case, you can use other Inventor tools to achieve the same result.

In this case, my two parts are already constrained along the center axis of each, so that the rod with the hemispherical face slides free toward the circular edge. So what I'll do next is create a Contact Set to be used with the Contact Solver tools. This allows me to slide the rod in until it contacts the other part, and it will stop at the exact point that the hemispherical face contacts the circular edge.

I do this by selecting both parts and then right-clicking and choosing Contact Set:

Parts involved in a Contact Set are denoted by a special icon in the browser. Here the last two parts are indicated as belonging to a contact set by the icon:

Then I'll go to the Inspect tab and turn on the Contact Solver:

Now that the Contact Set has been created and the Contact Solver has been enabled, I can drag the rod toward the other part until it touches, at which point it will stop and the hemispherical face will be touching the circular edge of the hole:

Now that it is in position I want to constrain it there. In this case I'll use a Flush constraint between a face on each part, and I'll make sure I enable the Predict Offset and Orientation check-box, so that I get the exact offset of the two faces as they currently exist in the assembly. In this case it's just over 106 mm:

So now my two parts are constrained perfectly:

Keep in mind that it's best to disable the Contact Solver when not specifically finding contacts between parts, because it might otherwise impact performance in a negative way as Inventor attempts to solve contact relationships while you drag other parts around in typical constraint and assembly tasks. Here's a link to another tip along with a video dealing withe the Contact Solver.

Also, remember that when you enable the Predict Offset and Orientation check-box it will stay on until you turn it back off. This can often be a source of confusion if you forget that you've turned it on, because your parts will constrain at their current offset rather than with a zero offset, as is more typical.

Contact Solver

Issue:

You want to setup your Inventor assembly so that parts will not pass through each other in an unrealistic manner.

Solution:

Add components to a Contact Set and then use the Contact Solver tool to allow Inventor to solve for contact. See video for how the tools work.

Note: It’s best to disable this feature when not specifically testing part contact, as it may impact performance in a negative way as Inventor attempts to solve contact relationships as you drag parts around in typical constraint and assembly tasks.

Inventor Video

ALT + Drag Assembly Constraints

Issue:

In past versions of  Inventor you used the ALT + Drag method to create assembly constraints, and employed keyboard shortcuts to allow you to change the constraint type. But now when you try it the ALT key highlights the Ribbon Keytips* as shown below, and does not allow you to enter the keyboard short cut to change the constraint type.

Solution:

When you see the Ribbon Keytips appear, let up on the ALT key and then press the ALT key again.

Procedure:

You can drag a component into position and automatically place a constraint (with no offset) by following these steps

   1. Hold down ALT, and then click the component to drag.

   2. Drag the component into position. As the dragged component nears the target component, the constraint is previewed.

   3. When the component is in the appropriate position, release the mouse to place the constraint. 

The type and solution of constraint you get depends on the geometry selected. For instance, when you drag a cylindrical part over another cylindrical part or hole, an inferred Mate constraint along the axes results. If you position the dragged part over a component face, Inventor infers a mate between planar faces.

   4. Change the constraint type by letting up on the ALT key and then pressing the ALT key again, then use one of these keyboard shortcuts:

M or 1 Changes to a mate constraint.
A or 2 Changes to an angle constraint.
T or 3 Changes to a tangent constraint.
I or 4 Changes to an insert constraint.
R or 5 Changes to a rotation motion constraint.
S or 6 Changes to a translation (slide) motion constraint.
X or 8 Changes to a transitional constraint.

The constraint glyph will change to indicate the current constraint type. If the geometry does not allow for one of the constraint types that Keyboard short cut is not offered.

*What are Keytips?

• Use the keyboard to access the Application Menu, Quick Access toolbar, and ribbon. 
• Press the Alt key or F10 to display shortcut keys for common tools in the application window. Keytips allow you to perform tasks without using your mouse. 
• When you select a keytip, more keytips are displayed for that tool. Keytips appear as underlined characters to indicate which key or combination of keys on the keyboard must be pressed to activate a command.

Keytips allow you to navigate in the Application Menu and in the ribbon using only the keyboard. Use the keyboard arrows to navigate to commands on the ribbon and Application Menu

Note: Keytips are not customizable.