Printer Friendly

Programming thread milling.

Milling is a great way to create a thread. Recall from last month's column that we discussed advantages of thread milling. Some people might be concerned with programming issues when thread milling. Well, let's look at a sample. The following program is designed to thread mill a 2.625x14 TPI internal thread using a 1" diameter multiple flute cutter with 3/4" flute length.

The plan is to position the cutter to the lowest point of the thread and feed out of the part. Our program calls for the tool to use a 45[degrees] ramp-in move, complete a 360[degrees] rotation within the part and then finish with a 45[degrees] ramp-out move.

For this program we are using the center of the threaded hole as the datum. At this point, the coordinates are X0, Y0. The first thing to calculate is the cutter start point called the "pivot" point. This can be calculated as follows:

Pivot point =(part diameter-cutter diameter)/2

Pivot point =(2.5"- 1.0")/2=0.750"

The cutter begins to cut the thread when the cutter is in this position (X0.750, Y0).

Although this is the point at which the tool begins cutting the thread, we must get the cutter to this point with a helical ramp-in move.

Use a point 45[degrees] from the datum point, midway between the X-axis and Y-axis zero line. This is half the value of the pivot point in both X and Y and represents the ramp-in start position. This is 0.75/2=0.375.

There are two advantage of this 45[degrees] start-point. First, the X and Y start and finish values are half the pivot point value. Second, we can easily calculate the amount of Z-axis movement required.

Calculate the Z-axis moves based on the required circular movement. The Z-axis move for a full 360[degrees] rotation is the pitch, pitch=1/14=0.0714"

We selected a 45[degrees] ramp-in move, so we can see that the Z-axis distance for this move will be 45[degrees]/360[degrees]x0.0714=0.0089.

Let's see how these values are used in the program. In this example the Z-axis start point is Z-0.50 and the milling method is climb milling.

In block N50 we feed to full depth and then move to the starting point for the ramp-in position. Remember that this is half the pivot point value.

The ramp-in move is a helical interpolation move with the X and Y axis moving incrementally 0.375 and Z moving 0.0089 upwards.

Look at line N70 and note that the ending Z absolute position is 0.0089 less than the starting point in block N50.

Block N80 cuts a 360[degrees] circular move using a negative I value. During this helical move the absolute Z value reduces by 0.0714.

Block N90 is the ramp-out position and again uses a 45[degrees] move in the X and Y axis with an incremental move of 0.0089.

I'm sure there are many thread milling methods out there. We hope this method is easy to follow and helpful in further understanding thread milling.

Steve Rose is a professional trainer and president of RTSI, Solon, OH. Rosaleen Rose offers Internet website development. They can be reached by phone at 440.542.3066; e-mail srose@; or on the web at
Program example

N10 T1 M 6 Tool change
N20 S1293 M 03 Spindle on
N30 G0 G90 X 0.0000 Y 0.0000 M08 Datum point
N40 G43 H01 Z0.1000 Rapid above part
N50 G1 Z- 0.50 F50. Feed to depth
N60 G1 X 0.375 Y-.375 F9. G41 D01 Ramp in start position
 G code for climb mill
N70 G3 X.75 Y.000 R.375 Z- .4911 F 5. Ramp in to pivot point
N80 G3 X .75 Y.000 I- .75 Z- .4196 Circle mill
N90 G3 X.375 Y.375 I-.375 Z-.4107 Ramp out
N100 G0 X.0000 Y.0000 G 40 Return to datum,
 cancel comp.
N110 G0 Z1.000 Retract from part
COPYRIGHT 2007 Nelson Publishing
No portion of this article can be reproduced without the express written permission from the copyright holder.
Copyright 2007 Gale, Cengage Learning. All rights reserved.

Article Details
Printer friendly Cite/link Email Feedback
Title Annotation:shop talk
Author:Rose, Steve
Publication:Tooling & Production
Geographic Code:1USA
Date:Apr 1, 2007
Previous Article:No sympathy for auto guys.
Next Article:Down Under burr removal: Ford Geelong/Victoria deburrs camshafts with Okuma, OrbiTool.

Related Articles
CNC speeds milling six-fold.
Tool training pays dividends.
Interpolation interpretation.
Tapping vs thread milling--where's the dividing line?
Innovative technique is what the doctor ordered: Florida firm relies on Traub machines for speed and accuracy.
Many ways to thread that hole: examine options carefully to maximize results.
+p high performance cutter slashes cycle time by 83%: faced with a challenging tapping application, a CNC job shop turned to a thread milling...
A soft spot for aluminum: as a soft metal, aluminum has many machining advantages, but its very nature can lead to unique challenges. Here are some...

Terms of use | Privacy policy | Copyright © 2018 Farlex, Inc. | Feedback | For webmasters