Tutorial: Timing Pulley Profile

This tutorial demonstrates profile machining operations to generate an HTD5 timing pulley.

This tutorial uses the new Plus Toolkit to generate the timing pulley profile.

Download the files used in this tutorial.

Step 1 - Insert an HTD timing pulley outline.

Use the new Plus Toolkit to generate a timing pulley by selecting the Toolkit - Timing Pulley menu item.

The plugin will prompt for the number of teeth for a 5mm pitch pulley, then insert a new curve with the center of the pulley about the origin.

A sample profile is available from the downloads file above.

ALT + double click will zoom the drawing to fit the view window.

Step 1 - Insert pulley profile

Step 2 - Insert a Profile machine operation

Select the pulley outline then click the profile machining operation button CAM Profile MOP from the toolbar. A new profile object will be created and displayed under the Machining folder in the drawing tree. The object property window will display the profiles's properties ready for editing.

Change the profile machine operation's properties to the following:

StockSurface 0
TargetDepth -5
CutFeedrate 200
PlungeFeedrate 100
ClearancePlane 1.5

Generate the resulting toolpath for the profile; right click the drawing to bring up the drawing context menu, then select Machine - Generate Toolpaths.

Step 2 - Insert Profile MOP

To rotate the 3D drawing view, hold the alt key then click and drag on the drawing. To reset the view, hold the alt key then double click the drawing. Another rotation mode can be set in Tools - Options, RotationMode = Left_Middle. If this mode is selected the view can be rotated by clicking the middle mouse button and dragging with the left. To reset the view in this mode hold the center mouse button and double click.

Step 2 - Rotating View

Step 3 - Creating the inner hole

First draw a circle using the cricle drawing tool Draw Circle with the center on the origin with width 8.

Select the circle and insert another profile machining operation CAM Profile MOP. Set the target depth and other properties to match the first profile operation. Change the InsideOutside property to Inside. Again, right click the machine operation in the file tree and Generate Toolpath.

Step 3 - Inside Profile


Step 7 - Creating G-Code

Before producing the gcode output, now would be a good time to save your drawing.

Visually inspect the toolpaths and double check the parameters of each machining operations.

To create a gcode file (post), right click to get the drawing menu then select Machine - Produce GCode.

CamBam will then prompt for the location of the gcode file to produce. If the drawing file has been saved the default file will be in the same folder as the drawing file with a .nc extension.

If the destination file already exists you will next be asked to confirm whether to overwrite it.

To control how the gcode file is produced, select the machining folder from the drawing tree. The machining properties for this drawing will then be displayed in the object properties window.

Copyright (c) 2018 HexRay Ltd