There was a discussion on the Fusion forum about being able to create a construction point that’s positioned at a specific X, Y, Z location. There is also a post on the IdeaStation. Fusion doesn’t currently support that capability but only supports the creation of construction points relative to existing geometry. When creating construction geometry, there are two situations to consider; capturing design history (parametric modeling) and not capturing design history (direct edit modeling). You switch between the two modeling types using the command in the context menu on the root component node in the browser, as shown below.
Direct Edit
In a direct edit design, construction points don’t remember their relationship to the original geometry used when creating them and they can be moved to any location after they’ve been created using the Move command. Using the Move command it is possible to end up with a construction point at the desired X, Y, Z location but it’s an inconvenient workflow to first create the point and then move it.
Parametric Model
When working in a parametric model, all construction points are dependent on other geometry and can’t exist anywhere in space so it’s not possible to position a point at an arbitrary X, Y, Z location. However, parametric designs support something called a “Base Feature”. A base feature lets you create an “island” of direct edit data within your parametric design, so it ends up being the same workflow as in a direct modeling design, except that you also need to first create a base feature, as shown below.
So, it is possible to create a construction point at a specific X, Y, Z location in both parametric and direct modeling designs, but it’s inconvenient in both. With the recent May 7 Fusion update, the API now supports the creation and edit of base features. With this capability it’s now possible to write an add-in that will support the creation of a construction point at a specified X, Y, Z location.
Once the add-in is installed, you’ll now see a new “Point at Coordinate” command in the CONSTRUCT menu, as shown below.
When you run the command when you’re in a direct modeling design the dialog on the left is displayed and when you’re in a parametric design, the dialog on the right is displayed.
Using the “Name” field you can specify what the name of the new construction point will be. The default is “XYZ Point” but sometimes, depending on how you’re going to use the point, it can be useful to name it so you can easily identify which one is which when looking at the browser.
The “X Position”, “Y Position”, and “Z Position” fields are the X, Y, and Z values where the construction point will be created. You can use any valid expression when specifying these values, including the use of parameter names. For example, if you have a parameter named Length you can use “Length/2”. The default units are whatever the current design units are. But you can also override that by specifying the units. For example “3 in” will be interpreted as 3 inches. Whatever you use as input, it’s important to understand the point doesn’t remember this relationship so that if you use a parameter name and then later change the parameter value, the point will not move.
When the command is run in a parametric design, the “Base feature” dropdown at the top of the dialog is displayed. Because points at an arbitrary location must be created within a base feature when working in a parametric design, this lets you specify which base feature they’ll be created in. If there isn’t an existing base feature, a new one will be created and that will be the default base feature when you run the command again, although you have the option of choosing any existing base feature.
To use the add-in just unpack the zip file anywhere on your computer. Run the “Scripts and Add-Ins” command and click the green “+”, as shown below. Browse to the location where you unpacked the zip file and choose the PointAtCoord.py file. You’ll only need to do this once because Fusion will remember it for subsequent sessions.
You can either shut down and restart Fusion to make the command available, or while in the same session you can start the add-in. This is only needed when first enabling the add-in because it will load automatically in subsequent sessions of Fusion. To start the add-in, choose the “Add-Ins” tab on the “Scripts and Add-Ins” dialog, select the “PointAtCoord” add-in from the list, and click the “Run” button.
Now, and in all sessions of Fusion the “Point at Coordinate” command will be available.
You can find the source code for this add-in and a few others here on GitHub. Please let me know if you find any problems or have suggestions on improvements.
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