'Using the User Defined 3+2 Machining Mode' Tutorial

This page provides step-by-step instructions to guide you through using the 3+2 Axis machining mode, with the ‘User-defined’ machining direction.

With this machining direction:

The tool orientation that CAM Assist uses to create the toolpath strategy can only come from the +X, -X, +Y, -Y, and +Z axes.
The tool then operates on the part from a fixed orientation, which means that the orientation cannot change during cutting.

Step-by-step instructions

Selecting a part and opening CAM Assist

CAM Assist works with the Siemens NX manufacturing environment and manufacturing templates.

Open CAM Assist - in the /wiki/spaces/CAFSNCUG/pages/145096925, click CloudNC CAM Assist.

Specifying the ‘3+2 Axis’ machining mode

For Machining Mode - select ‘3+2 Axis’.

For Machining Direction - select ‘User-defined’.

Configuring the ‘Target setups’

Ensure at least one ‘setup’ is checked.
- The content of the ‘Target setups’ section reflects the workpiece configuration of the part, as displayed in the 'Geometry View’ of the Siemens NX Operation Navigator.
- If you want CAM Assist to create a toolpath strategy for a setup, ensure that the respective setup's checkbox (such as 'Setup 1') is checked.

For each setup that you’ve checked:

Choose from the options shown in ‘User-defined’ options, below.
(Optional) Avoidance geometry - see Avoidance Geometry, below.

Optional - configure required parameters within CAM Assist’s other tabs:

Click OK.
- The CAM Assist UI closes.
- CAM Assist now computes a toolpath strategy for the part within Siemens NX.

‘User-defined’ options

The following table shows the options available for the 3+2 Machining mode (user-defined).

Option	Details	How to Use
Same direction for roughing and finishing	Checked - indicates you want to machine the part in the same direction for both roughing and finishing operations. Unchecked - indicates you want to machine the part using different directions for the roughing and finishing operations. If unchecked, the ‘Select machining directions' option is replaced with both ‘Select roughing directions’ and ‘Select finishing directions'	Check/Uncheck the checkbox.
Select roughing directions	These options are only displayed if ‘Same direction for roughing and finishing’ is unchecked. For this option, you can only select planar (not curved) faces on the Fusion part. You can select a cylindrical face that features a hole as a direction of tool orientation. You will not be able to click ‘Run’ until both directions have been selected.	Click on the block icon (to the right of ‘Select roughing directions'). On the Siemens NX part, select at least one face - you can select as many as required. ‘Select roughing directions (0)' changes to 'Select roughing directions (n), where n is the number of distinct faces selected. A green tick to the left of ‘Select roughing directions (n)' indicates the selected faces have been accepted by CAM Assist.
Select finishing directions	These options are only displayed if ‘Same direction for roughing and finishing’ is unchecked. For this option, you can only select planar (not curved) faces on the Fusion part. You can select a cylindrical face that features a hole as a direction of tool orientation. You will not be able to click ‘Run’ until both directions have been selected.	Click on the block icon (to the right of ‘Select finishing directions'). On the Siemens NX part, select at least one face - you can select as many as required. ‘Select finishing directions (0)' changes to ‘Select finishing directions (n)’, where n is the number of distinct faces selected. A green tick to the left of ‘Select finishing directions (n)' indicates the selected faces have been accepted by CAM Assist.
Avoidance geometry	(Optional) see Avoidance Geometry, below.
Keep roughing order	Checked - tool orientations will be ordered in the same sequence as they are selected (this applies to ‘Select roughing directions’, see below). Unchecked - tool orientation will be sequenced by CAM Assist but may not be in the order selected.	Check/Uncheck the checkbox.
Workholding security	Use the slider to set the ‘Workholding security’ for the specified setup. Excellent - a more secure ('excellent') workholding, such as a vise with serrated jaws, will result in CAM Assist selecting larger tools or more aggressive cutting parameters. This will result in faster toolpaths, but with more force on the workpiece. Poor - a less secure ('poor') workholding, such as a thin part held by a soft jaw, will result in CAM Assist selecting smaller tools or less aggressive cutting parameters. This will produce slower toolpaths, but with less force on the workpiece.	Move the slider to the required position. Based on the slider’s position, the ‘Largest available tool’ is the largest tool diameter that will be available by CAM Assist to calculate a toolpath strategy. CAM Assist will choose roughing tools suitable for the specific workholding.

Avoidance Geometry

This geometry ensures that machining operations do not occur in specific portions of the stock for this setup, such as the space under the part or between the vise jaws.

These blocked out portions (Avoidance geometry) are different from fixture bodies. While fixture bodies MUST be avoided, the Avoidance Geometry is considered part of the stock and may be gouged in specific cases. For example, drilling a through-hole may pierce the avoidance geometry but not the fixture.

Fixture bodies also require clearance from any tool, whereas all roughing tools may touch the surface of the Avoidance geometry.