Shop Doc – Polygon Milling on a Small Part

Todays Machining World Archives May 2008 Volume 04 Issue 05

Dear Shop Doc,

We are trying to make a part of beryllium copper that has a .025″ square pin on one side. The length of the square pin is .140″ long, then transitions to a diameter of .035”, and then to a shoulder at .150” diameter. The problem I am having is that we have to turn the raw material down to .035″ before we polygon mill the .025″ square. We’ve done polygon milling on much larger parts but this is our first time on a small part. We are using a CNC Swiss lathe that has opposing X- and-Y-axis gang plates that are controlled separately.

Poly Gone

Dear Poly,

I know exactly what you are trying to attempt. What you’ll need to do is adjust your methodology to account for the fact that you need to turn the raw material from .250″ diameter to .035″ and polygon mill at the same time. What is happening in your current method is that after you turn the .035″ diameter, the material is no longer supported by the guide bushing. To fix your problem, you need to turn the .035″ diameter at the same time you are polygon milling.

Two actions need to be taken:
1. Tooling: In the Z-axis plane, the turning tool needs to be closer to the material than the polygon tool. The reason for this is to turn the diameter before the polygon tool starts creating the fats. I know in most Swiss machines this is already built into the tool holder geometry where the live tools are typically further away from the guide bushing compared to the turning tools. If this is not the case, then you’ll need to make some physical adjustments so that you can set the tools properly – either by shimming the polygon tool or grinding the shank on the turning tool. Then find the distance between the two tools in the Z-axis plane. As an example we’ll use .010″ as the distance between the two tools.

2. Programming: To program this you’ll need to understand how to utilize tool offsets. For the turning tool, just program it in the normal fashion where you call the tool and the offset. For example: T0101 – Tool 01 and offset 01. For the polygon tool just call up the tool position without the tool offset. For example: T0200 – Tool 02 and no offset. For the G-Code, simply add the distance between the two tools to your programming of the turning tool to get to the linear dimension of the .025″ square.

In your particular component, (using the example of .010″) you’ll want to program your turning tool to .150″ in the Z-axis to account for distance between the turning tool and the polygon tool. This will give you the net result of producing a .025″ square that is .140″ long. If you need to contour the shape of the square, then the programming gets much more complex and you’ll do just the opposite of my example. You’ll have to use the polygon tool offset and omit the turning tool offset, then control the path of the polygon tool in the program. However, you’ll still need to keep the turning tool in front of the polygon tool and account for the difference.

Happy Machining!

David Cogswell
Regional Manager at Gosiger Inc.

Share this post