How To Use Custom User Coordinate Systems with Inventor Assembly


How To Use Custom User Coordinate Systems (UCS) with Inventor Assembly for Inventor Professional

The origin within an Inventor assembly or part is a feature not often thought of. The origin is assigned 3 planes, 3-axis, and a point that can be referenced throughout your file. The Inventor UCS feature allows professionals to use the same definitions as the origin on your part features and assemblies.


Placing and Defining a UCS – How Inventor professional can be useful within a part

Upon selecting the UCS feature, you are prompted to place it on a point. This point defines the origin of the UCS. You will be asked to select this x and y-axis afterward from two points. These two points need to be defined. If you set the UCS in space, it will be referencing its relation to the origin. A workaround for placing a UCS without having defined the x or y-axis is to right-click on your mouse and select finish. Each UCS creates 6 parameters, 3 translational and 3 rotational, in relation to the point that it was placed.

Each UCS is associated with 6 parameters to move it or rotate it. These are in reference to the orientation and point it is placed at (by default this is in reference to the origin point and orientation). Having the 6 parameters is useful when using them to define features and to move parts after being placed. These parameters are helpful when moving your UCS.


Another method to move a UCS is to select it either in the model tree or in the model, then dragging with your mouse on the axis to rotate or translate it. Your mouse pointer will indicate the movement depending on where it is when you start dragging. The delta for the movement will be indicated in the dialog box. You are also able to directly type in the value to the dialog box.

One example of a UCS use at the part level is with the hole feature. Once a UCS is placed, you can use its reference geometry as a reference for your hole. In the image below, a hole was placed on the edge of a round surface at a skewed angle.

Using a UCS within an Inventor assembly as a constraint

Constraining parts

Within Inventor assembly, a UCS can be used as a constraint that restricts movement in all directions. This constrains the 3 axes and the point of the two coordinate systems. To use a UCS-to-UCS constraint, use the Constraint Set tab within the constraint dialog box. When you use this, the second UCS you select will be the one to move to the location of the first one selected.

There are a few different uses for a UCS-to-UCS constraint. The first is to constrain two parts to each other. This is like the rigid constraint where it removes all degrees of freedom.  A second use for this constraint is redefining the origin of a part or assembly. If you have legacy parts or parts from a source outside your company, they might not have been created with the same standard origin as your company. This constraint will help relocate the origin of those parts to a more standard location.

Reorienting an Inventor assembly

An additional use for this constraint is to reorient your origin. By default, Inventor creates an origin with the y-axis pointing up. This is not the ideal orientation for all Inventor users. Using a UCS on a part, you can constrain it to the origin of a z-up assembly. This can be done by creating a UCS on your part or assembly at the location and orientation that you would like the new origin to be. You can then create a new assembly with an origin that has your desired orientation.

Place a UCS at the origin. If you set your desired home views, the new UCS parameters will just need to all be set to O. After importing your part, constrain the USC on your part or assembly and the UCS at the origin. This will reorient your assembly. Using parameters, you are still able to move the assembly after constraining it.

Check out the recent Autodesk Virtual Academy on the topic below for an even deeper dive!

Sign up for KETIV’s weekly webinar, Autodesk Virtual Academy to see more updates for Autodesk manufacturing software!

Leave a Reply

Your email address will not be published. Required fields are marked *

Check out more posts from KETIV

Autodesk Inventor Model States
This guide explores Autodesk Inventor Model States, focusing on their evolution from Level of Detail (LOD), the role of the primary model state, and their application in assembly environments. We highlight Model States' advantages in protecting intellectual property, improving design transportability, and providing precise information to stakeholders. The integration of Model States is deemed a game-changer, offering efficiency and enhanced capabilities to both seasoned and new Autodesk Inventor users.
How to Find Internal Volume in Inventor Professional
Knowing the internal volume of an object can help designers optimize its functionality and performance. If you need to determine the amount of space within an object that can be filled with liquid or gas, finding the internal volume using Autodesk Inventor is an essential feature. This tool can be useful for a variety of […]