Contour Operations Using Thread Mill Tools

This article explains the correct way to program Contour processes using Thread Mill tools: the "two-value" method. Then it goes on to talk about what happens to tapered thread processes that unfortunately use the "one-value" method instead. In the future, this article will also have an expanded discussion at the end on whether and how to fine-tune the start and end points.

Bottom line: In v10.3 tapered threading, the value for High Z must exceed the value for Low Z by at least half the thickness of the Thread Mill tool.



Because the Depths Diagram is used by many different processes, its fields have different names. In the Contour process, for most types of cutting, we say "Surface Z" or "Top Surface Z" for the lower-left value, and "Floor Z" or "Finish Depth Z" for the lower-right value. But in tapered threading, when the cutter follows a 3D space curve that might be an OD or ID, right-hand or left-hand, using Climb or Conventional, the usual labels become ambiguous.

For the purposes of this article, we call the lower-left value High Z and the lower-right value Low Z.


Always Specify High Z > Low Z when Contouring Tapered Threads

The following illustrations show correct programming for tapered threads:

CW Cutter ID, Conventional ID, Climb

Why is this article necessary?

In GibbsCAM 2012+ (v10.3), Contour operations now use the tool profile for Thread Mill tools, just as for other tools. This lets you use Thread Mill tools for chamfering, for example. But the most common reason to use a Thread Mill in a Contour operation is for tapered threading.

The toolpath generation behavior changed from v10.1 to v10.3. Although Contour's new behavior for Thread Mill tools is more flexible, more powerful, and more consistent with other tools, it is incompatible with the data in Contour processes created using the "one-value" method (described below). When such a part file created before v10.3 is opened in the current release, the data will be changed so that regenerated toolpath will reproduce existing toolpath.

However, no such automatic adjustment will occur in newly created Contour processes, and if a new Contour process is created using the "one-value" method, gouging will occur. Be sure to double-check your macros, *.prc process group files, and custom plug-ins to make sure they don't use the one-value method.

Don't Do This! (The One-Value Method - Same Z for High and Low)

Prior to v10.3, there was a quick way to program the process that did not respect the tool profile. This shortcut allowed you to program right-hand and left-hand OD and ID tapered threads without giving them much care. In v10.3, this method is no longer valid for programming tapered threads, even though the system will accept the values (because it doesn't "know" what kind of geometry you are following). Don't do this: