Swiss Screw 2D (22:42 min)

00:06

In this lesson, we'll be programming from a print using the part shown here.

00:15

To start, we'll need to open a Tools File and a Cycles File, so I'll go to File, open Tools File, and open a tools file.

00:27

Go back to File, open Cycles File and we'll open our cycles file.

00:32

The next thing is to save our job file to the same location as our tools and cycles files.

00:40

And I'll name that "Swiss_Screw".

00:45

So, the first thing that we need to do is go to our Setup dialog and setup the stock boundaries.

00:54

First, we'll set the length, which is going to be the final part length, which is 1.2 in this case.

01:03

We'll then go to the OD, which is going to be the stock material size, which will be a quarter inch.

01:08

The Excess Stock is the amount of material we're facing off the front of the part.

01:12

We're going to go with 15 thousandths for that.

01:15

The Guide Bushing Length, we'll go with 750 for our landing size.

01:20

And we'll set our Guide Bushing outer diameter to 1 inch.

01:25

As you can see right now, we only have one face window on our list of face windows.

01:29

We will always start with the Main Spindle turn and we're going to name this one to "Main Turn" and then will "Apply" and "Close".

01:40

To get started, we use the CAD/CAM Switch to switch over to our CAD side.

01:47

And we'll select the Connected Lines icon to start drawing.

01:52

Down in the bottom, we're going to start our first coordinate at (0,0) so we'll type in 0, we can tab over 0 and "Enter".

02:03

Our next coordinate is going to be X, 50 thousandths.

02:10

We'll then go to Z, 0.230.

02:16

We're then going to go in X to a 0.0874, which is our thread major.

02:23

We're then going to go in Z to 0.760.

02:30

In X, we're going to go to our largest diameter, which is 0.230.

02:37

In Z, we'll move to 1 inch.

02:42

In X, we'll go down to 0.208.

02:50

We'll move in Z to 1.1.

02:55

In X, we'll go down to 0.1455, which is the outside diameter of our hex.

03:04

And we'll go to 1.2 in Z.

03:09

And then back to 0 in X.

03:16

Now, we can apply our chamfers and add our angled lines.

03:23

So, first, I'm going to select the Chamfer icon and we're going to type in a 3 thousandths chamfer for the front of the part.

03:33

So, we'll zoom in on the front, select the first front intersection there to apply our chamfer.

03:42

We'll go back to the chamfer and type in 5 thousandths and select the back of the part to put a chamfer there.

03:52

Now, to put our 120 degree angle on, we'll select the Line on an Angle icon, and from our Snap Mode's toolbar, we'll select the End of an Element Snap Mode to give it a starting point.

04:09

We'll select our starting point and we need to type in our 120 degree angle and we'll click above the 0.230 diameter to snap our line to it.

04:23

We're going to do the same thing to start our thread.

04:26

So, first, we'll select our starting point.

04:33

We'll make sure we have a 120 in our angle and then we'll snap the line to its above horizontal line.

04:41

We can then grab the Remove icon and click on each of the segments that we want to remove.

04:53

We're then ready to mirror the part over the Z axis.

04:57

So, we'll click and drag a box around the part.

05:04

We'll select the Mirror icon.

05:08

We're going to use Multiple copies.

05:10

We're going to use the Horizontal Mirror Axis and we're going to press "Mirror" and "Close".

05:21

Using the CAD/CAM Switch, we'll switch back over to our CAM side to start creating our first facing operation.

05:29

To do that, we'll select a new Profile Group.

05:33

We'll choose a contouring strategy and change our Tool Location to Face.

05:40

We'll then uncheck Roughing and go straight to Finish and we'll select a tool.

05:45

We're going to select the 80 degree right handed turning tool, which is number 2 on our Gang Slide and we'll press "Select".

05:55

We'll then name this group "Face" and we'll "Apply" and "Close".

05:60

We can then verify our toolpath using the Verify Workgroup Toolpath button.

06:12

For our next operation, we'll turn back just past the threads.

06:17

First, we'll go ahead and select a new color and we'll press new Profile Group.

06:23

We're going to use the contouring strategy, Tool Location-Out and Tool Orientation-Right.

06:31

Again, we're going to go straight to Finish, so we'll go ahead and uncheck Roughing.

06:37

We'll select tools and we're going to use the same 80 degree right handed turning tool and press "Select".

06:43

And then we'll name this "OD Turn 1".

06:49

And we can "Apply" and "Close".

06:54

To chain this toolpath, we'll use the Define Profile icon.

06:59

And from our Snap Mode's toolbar, we'll select the End of an Element Snap Mode.

07:05

I'll zoom in on the front of the part and will select the bottom of the 3 thousandths chamfer and work our way up to the major diameter of the thread.

07:14

Now, we want to go exactly back to 0.450, so from our Snap Mode's toolbar, we'll select the ZX Coordinates Snap Mode.

07:23

Down in Z, we can type in 0.450 and "Enter".

07:27

Now, we're going to want to get out of the stock, so we'll type in X, 0.250, to go back to our stock diameter.

07:36

Now, we can go ahead and verify this toolpath using the Verify Workgroup Toolpath button.

07:44

And we'll press "OK".

07:54

Then we'll hide every toolpath.

07:58

Now, for our next operation, we're going to move onto our threading operation, so we'll choose a new Profile Group, Strategy will be Threading.

08:09

Now, the first thing that we'll do is select a tool to preset a few of these fields, so we'll select our threading tool, number 3 on the gang.

08:20

The first thing that we'll do is set our pitch.

08:23

Now, our pitch here is 56 threads per inch, so in Pitch, we'll type in 1/56.

08:32

If we delete everything in Thread Height, PartMaker will calculate the thread height as a factor of 0.6 of the pitch.

08:45

Our First Infeed is going to be the amount of material we take on our first threading pass, for that, we'll type in 5 thousandths, and Minimal Infeed, the minimum amount of material that we'll take per pass, we'll go with 1 thousandths for that.

09:03

The Acceleration Distance is going to be a multiple of our pitch, it's essentially our thread lead-in, so I'll take our pitch and we'll copy that and put it into our Acceleration Distance and then go ahead and multiply that by 3.

09:21

Now, this part doesn't have a thread relief groove, so we'll go ahead and Chamfer on Exit.

09:28

For our Chamfer Length, we'll go ahead and set that to our Pitch.

09:37

And it's going to exit at a 60 degree angle.

09:42

If you'd like a definition of any of these fields, select "F1" on your keyboard to open the Help dialog.

09:49

Let's go ahead and name this group "Threading" and we'll "Apply" and "Close".

09:57

Now, to chain this toolpath, we'll use the Define Profile icon.

10:01

We'll switch to our End of an Element Snap Mode and will select our first point.

10:09

For our second point, we'll switch to ZX Coordinates Snap Mode and type in exactly 0.450, which is where the end of the thread is.

10:19

And let's verify that toolpath.

10:37

Now, we're going to turn all the way back from the thread to the end of the part, so we'll create a new Profile Group.

10:44

The Strategy, again, is going to be Contouring, Tool Location-Out and Orientation-Right.

10:49

We're going to go straight to finish and we'll select the same OD turning tool.

10:60

Our group name is going to be "OD Turn 2".

11:04

Now, for this one, we want to blend into the cut, so we're going to go to our Leads and we'll make our arc radius 50 thousandths, line length 20 thousandths, and we'll give it a 45 degree angle to enter on.

11:22

Now, for leading out, we'll exit at a 45 degree angle, so we'll go ahead and give it a line length of 50 thousandths and an angle of 45 degrees.

11:36

Again, we'll choose the Define Profile icon.

11:40

And this time, we're going to use the ZX Coordinates Snap Mode to snap to an exact point.

11:46

So, we'll start at Z, 0.450, X, 0.0874 and since those are already in the brackets, we can just press "Enter".

11:56

We'll then switch to our End of an Element Snap Mode.

12:04

Now, to create a line going horizontally all the way to the back of the part, we'll choose the Horizontal Constraint and hover our mouse over the very back of the part and then we'll click.

12:18

Let's verify that toolpath.

12:24

To machine the steps on the back of the part, we'll first start by selecting a new color and we'll choose a new Profile Group.

12:32

Again, we're going to go with the contouring strategy, but this time, we're going to go with a left hand tool orientation and use a left-handed groove tool.

12:44

We'll uncheck Roughing so we can go straight to Finish and we'll "Select Tools".

12:50

Under Tool Type, we'll choose the Grooves tool type, and we're going to choose our Back Turning tool, which is number four on the Gang and we'll press "Select".

12:60

And let's give that a name, "Back Turn" and will press "Apply" and "Close".

13:07

Again, we'll choose the Define Profile icon with the End of an Element Snap Mode, and we'll select the points on the steps stopping at the top of the 5 thousandths chamfer and verify our toolpath.

13:22

For our last main spindle turning operation, we'll choose a new Profile Group and we're going to choose the Cutoff strategy.

13:31

We'll first select our tool, choosing the cutoff tool, number 1 on the Gang and press "Select".

13:39

We'll set our chamfer size to 5 thousandths.

13:42

Our start X point is radial, so we'll put in 0.1455 and divide that by 2.

13:52

We're going to press Optional Path 1-2-1 to cut to the bottom of the chamfer, lift up, chamfer, and then fully cutoff.

14:01

And then we'll name this group "Cutoff" and "Apply" and "Close".

14:06

We'll then verify that toolpath.

14:12

Now, if you want to change any group colors, you can simply right click on the name of it in your Job Explorer to change colors.

14:19

So, we'll go ahead and change a couple of these.

14:23

To mill the hex on the back of this part, we're going to have to go ahead and create a new face window in the Setup dialog.

14:30

We'll press "New" and from our Machining Functions list, we'll select the Mill Polygon.

14:37

I'm going to rename that to "Mill Hex".

14:41

And we can "Apply" and "Close".

14:46

You'll notice now that there's no drawing in our CAD window, that's because each face window is going to have its own CAD drawing.

14:54

So, what we need to do is switch over to the CAD side using our CAD/CAM Switch.

15:01

And we'll select the Polygon icon to draw our hex.

15:06

From the print, we can see that the Flat to Flat is 126.

15:11

We already have 6 sides in this dialog, so we can just press "OK".

15:17

We'll then select the CAD/CAM Switch to go back to our CAM side.

15:22

We'll press "New Profile Group".

15:24

First, we'll set up the Z position of the hex, setting that to Right Tool Edge and our P3 value will be 1.1.

15:34

Our X_Surf is a radial value, so we're going to type in 0.1455 and we'll divide that by 2.

15:45

Lastly, for our tool, we'll select a tool diameter of 0.156 and we'll press "Select Tools".

15:58

We'll select the 0.156 End Mill, number 7 on the Gang, and we'll press "Select".

16:05

I'm going to call this "Hex" and we will "Apply" and "Close".

16:11

Now, to put a toolpath chain on this, we can use the Chain Geometry icon because this is a closed loop, so let's select that, and we can select any point on the hex.

16:23

So, we'll click on the top right and we'll go ahead and chain our hex.

16:33

Once we verify, you'll see that these solid lines are the cutting moves and the dotted lines are the indexing moves.

16:43

Now, for our last operation, we'll go back to the Setup dialog, add a new face window, and choose a Turn function and Sub-Spindle, and this will be for the sub-spindle tapping.

16:57

I'll call that "Sub Turn" and will "Apply" and "Close".

17:14

Let's turn on our boundaries and axes so that we can see where our hole is going to be on the part.

17:20

We'll press "New Hole Group".

17:28

We'll set the Major Operation Type to Tap and set our Diameter to 60 thousandths.

17:36

Our Chamfer size is 10 thousandths and our Nominal Depth is 200 thousandths.

17:46

Then we need to add a cycle to this hole-making operation, so we'll press "Cycle".

17:51

Now, we already have a cycle in here, but we'll go through the process of creating it from scratch.

17:55

So, let's press "Add New Cycle".

17:60

Right now, we only have the Tap in here because that's the major operation we chose.

18:04

But we'll go ahead and click Insert Operation two times so that we can add a Spot Drill under drill, so we'll choose "Spot Drill", Spot Face for the Canned Cycle and then we'll choose "Drill" and a Drill Canned Cycle, which is just a single plunge.

18:21

If we delete the value in the Spot Drill hole diameter, we can search for all spot drills available in our tool library, so we'll do that.

18:29

But we know that our drill that we want is an 048 drill, so we'll type that in for Hole Diameter and let's press "Select Tools".

18:38

So, it looks like for our sub-spindle, we have an eighth-inch spot drill, so let's select that.

18:44

We'll select our 048 drill.

18:50

And we'll select our "Tap".

18:54

Now, the last thing that we need to do is set the hole diameter in our spot drill to the hole diameter of the Tap.

19:01

So, we can tell what size its chamfering on.

19:07

Then we'll press "Apply" and "OK".

19:11

You can see the spot drill is going in a depth of 40 thousandths based on our chamfer size of 10 thousandths.

19:19

And we can "Apply" and "Close".

19:21

Since we're in a turning face window, the operation is already on center, so we do not need to select any geometry to tell the tool where to go.

19:30

Now, we're ready to go to our Process Table to order our operations, synchronize our main and sub-spindle, set our pickoff, simulate and finally to post code.

19:42

Let's press "Generate Process Table" to get to our process table, we'll press "OK" and let's first look at the order of operations.

19:52

So, we're starting with our face, first turn, threading, second turn, back turning the steps, milling the hex and then our sub-operations.

20:03

You'll notice the cutoff is less than the process table and this is correct so that we can synchronize our main and sub-spindle.

20:11

From the Time Chart, you can see that the main spindle and sub-spindle are currently separate.

20:15

So, we'll go to our first mode switch at the very top of our screen.

20:20

Our main spindle mode's already machining with one tool, but we can tell our sub-spindle mode to machine with one tool as well, and modify for all consecutive processes which will set the rest of our main spindle processes.

20:34

Now, we need to do the same thing for our sub-spindle processes, so we'll click on the first Sub-spindle Mode switch and set our Main Spindle Mode to machine with one tool, and the subs already machining with one tool and we'll modify for our processes and press "OK".

20:49

Lastly, we need to set the pickoff for our cutoff operation, so we'll select the Cutoff Operations mode switch and set the Sub Spindle Mode to Follow Support and give it a 1-inch grip coordinate and press "OK".

21:04

Now, we can press the Synchronize button and on the Time Chart, you can see now the main and sub-spindle operations are overlapping.

21:12

The \E that you see next to the last sub-spindle operation automatically shows up anytime you create sub-spindle processes.

21:19

It will set the Eject to the last sub-spindle process.

21:24

Now, we're ready to go to simulation, so let's press the Simulation button and view our simulation.

21:45

Once our simulation is done, we can press "Show Finished Part" to view our part.

21:51

To post code, we need to go to the Job Optimizer and make sure we have a post loading, so we'll go to "Post Config File=?" and make sure that we have a post.

22:01

Right now, we already have our demo post loaded, but this is where you would search for your post processor.

22:08

And then we'll go back to Job Optimizer and press Generate NC Program.

22:13

Bringing up the Post Options dialog where we can type in our program number, bar load subprogram number, spindle speed limits, and other various options.

22:23

We'll press "OK".

22:26

Choose a save location, name the file and press "Save".

22:32

PartMaker then shows us our generated NC program.