The EZPath control is based around a conversational programming style. The use if the functions allow programs to be easily and quickly created as well as allowing for very quick single operations. The main screen of the control is shown above. From here you have many options. The control i will go over, is from the EZPath S model. If you have the EZPath 1, EZPath 2, or EZpath SD models, your control screen may appear differently, as they had some different options.

Here is a brief overview of the control, and some of my personal preferences of how to use it.

It is good to note that these machines operate in DIAMETER MODE. So if you move the tool 0.005″ as indicated by the digital read out, you will see a 0.0025″ actual movement of the tool. 

I have obtained a few of the Bridgeport operations manuals for different versions of this lathe. If you would like to download a copy of them, they are available on the information page.

MDI Menu

From the main screen, pressing “8” will enter the “MDI” menu.

MDI is where programs are written. 

We will take a look at how the functions of MDI are used to create a simple part. There are many features that are huge time savers, when programing complex geometry. 

Example Part

This is the part that we will program. Its a relatively simple part, but will display some of the time saving features of the EZPath control. 

When programming a part there are some considerations that need to be taken into account, Such as the tool geometry and order of operations.

Another thing to keep in mind, is the profile outlined in red is the profile that we will be programming. 

When programming arcs, Clockwise (CW) is as noted in red and green.

CW/CCW is defined from tailstock to chuck, on the operator side of the part.

It is important to reference the correct portion of the part when defining paths.

Click image to enlarge.

When programming a part, it is important to keep note of the order of operations, and the tools needed to cut each feature.

You define the shape of the part using a Path, then assign roughing and profiling operations to that path. This allows you to program complex geometry.

A part such as this should not be programmed in a single path, as demonstrated in the image to the right.

The profile of the part will be turned using a standard turning tool, but the groove, will need to be turned with a grooving tool.

Instead, program the profile of the part, excluding the groove, this way the roughing and finishing operations will ignore the groove.

Click images to enlarge.

Instead, program this part using two paths. Each path will define the portion of the part that each tool will cut.

One path for the main profile, and another path for only the groove as shown to the right.

You can use the backslash “/” key to open the view geometry menu, and entering the line numbers will display the programed paths for that section of the code. 

The image shows the result of each path that was programed.

Click images to enlarge.

When programing paths, there are really convenient ways to program fillets and chamfers using the Blend Line functions.

A blend line, inserts the chamfer/fillet at the end of the line, at the designated size and in the case of a fillet, direction.

Instead of having to program many small segments of lines, or arcs using a Blend Line combines that into the previous segment. 

This also saves needing extra dimensions on prints.

For example, the images on the right show a .125″ chamfer, and radius placed into a part in one command using Blend Line.


Click images to enlarge.

Once the paths are defined, we will utilize the tools programed in the library above to program the cutting operations for this part. 

We also need to program moves to ensure the operations are started from a safe position to avoid crashes.

The first operation is the roughing operation using tool #1.  

Pressing “F2” it opens the roughing operation menu. Here we need to enter whether the operation is an inside or outside diameter operation, as this operation can be used for boring aswell.

Next is the finish allowance, or stock to leave. This stock to leave will be what is left for the finishing Profile operation that is next.

Click the images to enlarge

After you enter your feedrates and stepover, there are three more options at the bottom.

The first is Cut Direction. This refers to cutting TOWARDS or AWAY from the chuck.

The Second is Undercut. The control will analyze the toolpath created, and check if the programed to will actually be able to follow the path created. If it cant, due to the geometry programed, it will throw a warning, and modify the toolpath when enabled.

The third, is auto rounding. The control will automatically round corners, using compensation for the nose radius of the tool, to create a sharp corner, but maintain smoother motion. Instead of moving to a sharp corner, it will rounds it instead. Examples of these conditions can be found in the images to the right.

Click the images to enlarge

The next operation is the Profile operation.

this is very similar to the roughing operation, but it is the finishing pass for the profile of the part. Most of the options are the same. Typically the feedrate is slower for a better surface finish. 

After programing the Roughing and Profiling operations, you can press the “*” key to verify the toolpath. 

This will plot the toolpath on the part and also check for undercuts. If the toolpath looks good, then the path and operation are defined correctly.

Click images to enlarge.

The only operation left to program is the Grooving toolpath. For this we use the grooving tool programed earlier as Tool#2. 

This will be programed to cut the profile defined in path #2. 

After filling in the feed and speed, this operation can also be verified using the “*” key. 

Notice the grooving tools position in the toolpath.

The “ZERO” point of the tool, is the chuck side sharp corner of the insert. The X Zero is the face of the insert, and the Z Zero is the chuck side face of the insert.

This causes the grooving toolpath to look somewhat strange, but the control is compensating for the programed width, and corner radius of the grooving tool. 

Click the images to enlarge

Once all of the captions are completed, the correct clearance moved, tool changes, spindle speed commands, and coolant commands are in place, the finished code should look something like this.

0000 EZPATH|SX 1 MODE|INCH MON JAN 16 23:41:24 2023
0020 RAPID ABS X0.0000 Z0.0100
0030 LINE ABS X0.0000 Z0.0000 F0.0100
0040 LINE ABS X1.0000 Z0.0000 F0.0100
0050 BLEND|LN ABS X1.0000 Z-0.5000 R0.1250 CCW F0.0100
0060 BLEND|LN ABS X1.7500 Z-0.5000 R0.0500 CW F0.0100
0070 LINE ABS X1.7500 Z-2.1250 F0.0100
0080 ARC|RADIUS ABS CCW X2.0000 Z-3.1250 R4.0625 F0.0100
0090 LINE ABS X2.0000 Z-3.6250 F0.0100
0120 RAPID ABS X1.7600 Z-0.8240
0130 LINE ABS X1.7500 Z-0.8240 F0.0100
0140 ARC|RADIUS ABS CW X1.7000 Z-0.8750 R0.0500 F0.0100
0150 BLEND|LN ABS X1.5000 Z-0.8750 R0.0500 CCW F0.0100
0160 BLEND|LN ABS X1.5000 Z-1.6250 R0.0500 CCW F0.0100
0170 BLEND|LN ABS X1.7500 Z-1.6250 R0.0500 CW F0.0100
0180 LINE ABS X1.7500 Z-1.6760 F0.0100
0190 LINE ABS X1.7600 Z-1.6760 F0.0100
0210 SETRPM S2000
0220 RAPID ABS X3.0000 Z5.0000
0230 TLCHG I1 T01 01
0240 AUXFUN M8
0250 RAPID ABS X2.1000 Z0.1000
0260 ROUGH 1 I1 X0.0050 Z0.0050 F0.0100 0.0100 0.0100 S0.0500 C0.1000W45.0000W0.0500D2U1A1
0270 RAPID ABS X2.0000 Z0.1000
0280 PROFIL 1 1 X0.0000 Z0.0000 F0.0100 C0.1000 E45.0000 W90.0000 U1 A1
0290 RAPID ABS X2.0000 Z0.1000
0300 RAPID ABS X3.0000 Z5.0000
0310 AUXFUN M9
0320 TLCHG I2 T02 02
0330 AUXFUN M8
0340 RAPID ABS X2.0000 Z0.1000
0350 RAPID ABS X2.0000 Z-0.8750
0360 GROOVE 2 3 A0.0020 F0.0100 R0.0100 P0.0000 C0.1000 O80.0000 L0.0000 D0.0000
0370 RAPID ABS X2.0000 Z0.1000
0380 RAPID ABS X3.0000 Z5.0000
0390 AUXFUN M9
0400 AUXFUN M0