Swiss Plug Solid Model (29:08 min)

00:10

The first thing that we're going to do is go ahead and open up a tools file.

00:16

So, I'll go to File, Open Tools File, and then I'm going to select the swiss2.tdb.

00:23

We then going to go to File, Open Cycles File and open the matching cycles.

00:31

Lastly, I'm going to go to File, Save Job File and we're going to go ahead and save that in the same folder.

00:37

I'll call it "swiss_plug" and we'll "Save".

00:42

The next thing I want to do is import a model, so I'm going to go back to File, Import and choose the X_T Parasolid File.

00:51

I'll pick my swiss2 plug and "Open".

00:59

Now, looking at this model, we can see that the origin set to the back of the part, not on the front, where we want our machining origin to be, we can also see that the blue line, which represents the Z axis, is not facing lengthwise across the part.

01:17

So, we'll have to go ahead and set our origin.

01:19

Let's select the Edit Part Coordinate System button, press "Set Part Origin" and select the Arc/Circle Center selection.

01:30

We'll press an arc on the front of the part and press "Set".

01:35

Next, I'm going to hit View Normal of face plane and we can see that the part is still not oriented correctly.

01:43

So, what we're going to do is go into rotate part, and we'll rotate around the X axis by 90 degrees and we'll hit Rotate until it shows up in the correct orientation.

01:54

So, this is what we want, origin on the right hand side, part on the left, and we'll "Close".

02:01

Our next step is to use the Extract Turn Geometry icon to take a section of the part.

02:06

This will also set our boundaries in our Setup dialog.

02:10

So, using sectional geometry, we can see that this section is not through the correct side of the part that we want.

02:16

So, let's go ahead and turn that 45 so that we don't turn away any milled features.

02:23

And press "OK".

02:27

Now, if we look up into our 2D window, we can see the section of the part shows up there.

02:33

If we go into our Setup dialog, the length was taken from the part length of the model, the OD was taken from the largest OD it could find.

02:43

So, we're going to change that OD to a half inch to represent our stock material.

02:48

We'll then set up our Excess Stock, the amount that we're facing off is 15 thousandths.

02:55

And our Guide Bushing Length and Guide Bushing Diameter 0.750 and 1 inch respectfully.

03:01

We're going to rename this to Main Turn.

03:03

We're always starting with the Main Spindle term window and we'll press "Close".

03:08

I'm going to start a new Profile Group for our first operation, which is facing the part.

03:12

We're going to select the contouring strategy of facing location, uncheck Roughing, so we go straight to Finish, and we'll select and an OD Turn 80 Right tool, which is number two on our Gang.

03:29

The group named for this, we'll call it Face and let's "Apply" and "Close".

03:36

Let's go ahead and verify that toolpath.

03:39

We'll set our Verification Delay to 3 and we'll press "OK".

03:45

We'll press "Hide Every Toolpath".

03:49

For our next operation, we'll start the ID features, which we have to drill and then bore this out.

03:57

So, let's start a new hole group and using the model will extract geometry from the model to get the information for hole size and depth.

04:08

So, from our selection, let's choose Select Holes.

04:12

We'll select the inner diameter of the hole and we'll press "Extract".

04:19

Now, we already have a cycle created in here from our Cycles File, but we'll press "Add New Cycle".

04:29

Let's go ahead and insert an operation so that we can do a spot and a drill.

04:33

We'll add a Spot Drill-Operation Type and a Spot Face-Canned Cycle.

04:38

I'm going to delete the information from our spot drill hole diameters that we can search for all spot drills in our library, and we'll press "Select Tools".

04:47

We have one called Spot Drill Main that's on our end-working slide, let's press "Select".

04:54

And our drill, which is also on the end- working slide and we'll select that.

04:59

Now, the last thing we need to do is set the hole diameter to match our drill diameter for our spot drill.

05:06

So, we'll call that 120 and this is so that it knows what size hole its chamfering on.

05:12

We'll then press "Apply" and hit "OK".

05:17

If we deselect Extract Parameters from Solid, it will allow us to edit any of the parameters in the Hole Group Parameters dialog.

05:25

Since this chamfer is actually being done by the boring bar, we're just going to put a one-thousandths chamfer into the Chamfer dialog to open up the hole.

05:35

We'll press "Apply".

05:38

Let's go ahead and verify this toolpath in 3D using the single step button at the bottom.

05:50

We have our spot drill and our drill.

05:55

Now, let's move back up to the 2D window and we're going to press "Show holes in profiles for workgroup only", and what that allows us to do is to only see the profile group that we have selected in the Job Explorer on the screen.

06:10

So, let's select a new color and we're going to go ahead and use the solid model to create our ID boring operation.

06:22

So, let's select a new Profile Group, Strategy-Contouring, and we'll set Tool Location to In.

06:28

We'll uncheck Roughing to go straight to finish and we'll select the ID boring bar that we have in our library, and you can see that's on our end-working slide.

06:40

I'm going to name this ID Bore and we'll "Apply" and "Close".

06:46

Now, to select our geometry, we can use the Define Profile on Solid Model icon.

06:51

Once we press that, it will section the part for us and then we can select points directly off of the model.

06:59

So, I'll select the following points and we'll single step to verify this toolpath.

07:06

The next thing to do is to open up the ID BORING dialog again, and we're going to set a cutting point to make sure that the tool pulls out on Z before it moves back up in X.

07:17

So, we'll select Return to Cutting Point.

07:19

We'll set a User Defined point and I'm going to put Z 10 thousandths in front of the part and we're going to move X to 0.180, and we'll press "OK" and let's see where that takes us.

07:32

So, again, we're going to single step our toolpath.

07:38

And now we see we have a movement taking the tool out of the part before it goes back up in X.

07:55

For our next operation, we're going to turn the OD right past the thread relief groove, so we're going to choose a Contouring-Strategy, Tool Location-Out and Right.

08:04

We'll select Finishing and select our OD Turn 80 Right tool.

08:10

For the group name, I'm going to call this OD Turn 1.

08:14

And we'll "Apply" and "Close".

08:19

This time, what we'll do is go ahead and select this off of the 2D.

08:24

So, we're going to use the Define Profile icon with the End of an Element snap mode and we'll select the following points.

08:32

Now once we get to the top diameter of the thread, we're going to use the horizontal constraint to take us all the way to the back of the thread relief groove, and then we'll go up.

08:42

Now, if we want to manually take the toolpath out of the part, we can switch to the Z-X Coordinates snap mode, go into X, and I'm just going to type in the part diameter half inch and then let's verify that toolpath.

09:14

For our next toolpath, we'll go ahead and create the Thread Relief Groove, so we'll start a new Profile Group, from strategy, I'll select "Grooving".

09:24

And first, we'll select the tool, we'll select the grooving tool, number four on our Gang.

09:30

Now, the grooving strategy has two different profile shapes, so we have rectangular, which is just simple groove shapes and then we have general, which allows you to do a rough and finish.

09:40

It also allows you to choose from inside to side roughing or side to side, so this would be for more complex grooving shapes.

09:47

We're just going to stick with rectangular for this one.

09:50

I'm going to name it Groove and let's "Apply" and "Close".

09:56

Let's choose the Define Profile icon and the End of an Element snap mode from our Snap Mode's toolbar, and we're just going to pick the four points outlining the groove and we'll verify the toolpath.

10:13

We can also verify this in 3D once we've created the operation.

10:30

For our next operation, we're going to create a new Profile Group and we're going to choose the Threading Strategy.

10:38

So, first, we're going to go ahead and select a tool.

10:44

Now, we're going to set the Pitch, so for this, it's 28 threads per inch, so we'll type in 1/28.

10:51

We'll delete everything in Thread Height so that PartMaker calculates the thread height on its own as a factor of the pitch.

10:59

For our first infeed, which is our first depth of cut, we're going to go with 5 thousandths, and for minimal infeed, we'll go with 1 thousandths, so that's the minimum material we're allowed to take.

11:10

We'll press "Apply" to calculate everything.

11:12

And the last thing, we're going to change the Acceleration Distance, so it's essentially our thread lead-in.

11:19

We'll take our pitch and copy it and we'll paste it into there and then let's multiply that by 3.

11:28

And last thing, let's just give this a group name, we'll call it Threading.

11:34

And we'll "Apply" and "Close".

11:39

Let's select our Define Profile icon and End of an Element snap mode.

11:45

And for our first point, we're just going to select our first thread.

11:51

And we want to move horizontally over into the thread relief groove.

11:54

So, one way to do this is to select the Screen snap mode and the Horizontal Constraint at the same time, and we'll just pull that line over until we're just past the end of the threads, but not too far so that we hit the wall of the thread relief groove.

12:10

So, we'll go ahead and click and verify the toolpath to make sure it doesn't hit the wall.

12:25

For our next operation, we're going to turn the OD the rest of the way back, and we can do this one on the Solid Model, so we'll select a new Profile Group.

12:34

From Strategy, we'll select Contouring, Tool Location-out and Tool Orientation-Right.

12:40

I'm going to go straight to Finish again and we'll select the 80 Degree OD Turning tool.

12:49

And I'm going to name this one "OD Turn 2".

12:54

And "Apply" and "Close".

12:56

So, for this one, we'll choose the Define Profile on Solid Model icon.

13:04

And I'll select the following points and we'll stop at the top of the chamfer that will end up doing with our cutoff tool.

13:14

Now, if we want to move manually out past the end of the part, we can use the X Coordinate snap mode.

13:19

We can use the "@" symbol and add a distance, so we'll go with 120 and press "Enter".

13:24

So, the "@" symbol is actually an incremental movement and then we'll do "@" in X and we'll go up just 50 thousandths.

13:33

And press "Enter".

13:36

So, let's go ahead and verify that with the single step button.

13:55

For our last turning operation, we're going to go with a cutoff strategy and we'll select our Cutoff Tool first.

14:06

The chamfer on this part is 10 thousandths and since we're turning the OD down to 480, we're going to put a Start X Point of 0.240.

14:20

I'm going to select Optional Path 1-2-1 so that we cut down to the bottom of the chamfer, lift back up, chamfer, and then cutoff, and then we'll name that cutoff.

14:30

And "Apply" and "Close".

14:32

PartMaker generates the toolpath for us if it's a cutoff operation and let's use the single step to view this toolpath.

14:49

For our first milling operation, we're going to use a sliding saw to cut the slot in the front of this part.

14:54

But before we do that, let's take a quick measurement from the model to see how thick our slot solid needs.

15:00

So, we'll press the Measure Solid Model icon and I'm just going to select two points on the model.

15:08

So, we can see the distance that is 40 thousandths, so we need a 40 thousandths thick saw.

15:15

Now, if we want to measure how far back in Z this goes, we can just double click on the back face.

15:23

We see that the Z offset there is also 40 thousandths.

15:32

Since we're moving to a milling operation, we need to go to our Setup dialog.

15:36

Create a new Face window and our Machining Function for this one is going to be a Mill Z-Y plane, and that's because the shank of our tool is facing in the X direction and we're moving with the Z and Y coordinates.

15:49

So, let's go ahead and call that Mill Slot and we'll "Apply" that.

15:53

And before we do that, let's take a quick look at the model and make sure that we're facing normal to the correct side of the part.

16:01

So, let's select the View Normal to Face Plane icon.

16:10

Now, looks like in this case, we are normal to the correct section of the part.

16:15

However, if we needed to rotate the part, we'd use the Index Angle(C) within the Setup dialog, type in our angle, "Apply", and then check with View Normal to Face Plane.

16:27

Now, this is the correct way to rotate the part around within the software.

16:31

Once you've set the origin in the beginning of your program, you do not need to rotate or set your origin again.

16:49

Now we know that the slot needs to be 40 thousandths in the Z axis, so for our toolpath, we really only need a straight line for our slot, so let's go back to our 2D window.

17:03

We'll turn on our boundaries and axes.

17:06

And let's go to the CAD side.

17:11

I'm going to pick the line parallel to the Vertical Axis icon, and we can create a line at 40 thousandths in in the Z axis, and that's going to represent our toolpath.

17:24

Let's create a new Profile Group.

17:27

The strategy we want is a contour milling strategy with tool position either left or right.

17:33

If we choose left, it's going to climb cut.

17:35

If we choose right, it's going to conventional cut.

17:38

So, we're going to go with left.

17:40

First thing, let's uncheck Roughing, go to Finish and we'll "Select the tool".

17:45

So, if we press Select Tools, we'll choose from Tool Type, slot mill, and we'll press All Diameters to see what we have in our library.

17:55

So, we're going to choose this half inch diameter slot mill.

17:58

The next thing we need to do is set our X_Surf and our X_Depth.

18:02

So, to get to the center line of our part, we're going to choose an X surface of 0, however, for our X_Depth, we're going to need to drop the tool down by half the thickness of the tool.

18:14

So, we'll type in 20 thousandths into X_Depth.

18:20

I'm going to name this Slot Mill and we'll "Apply" and "Close".

18:26

Let's use the Define Profile icon with the End of an Element snap mode

18:29

and we're just going to select from top to bottom and we'll verify our toolpath.

18:42

We can also verify this on the 3D model to make sure that it's going through the right place.

18:52

Now, if you need to reverse the direction of the line, select the line and press the Reverse icon, and verify again to make sure that you're on the correct side of the line.

19:11

Next, we'll go ahead and mill the flats on this part.

19:16

So, for that, we're going to go to the Setup dialog and we'll create a new Face window.

19:20

We're going to go with another Mill Z-Y Plane because we're using an X-oriented tool, moving the tool in Z and Y.

19:29

We're going to call this one "Mill Flats".

19:34

But this time, we're going to use the duplicate function.

19:36

So, any operation created under this Face window is going to be duplicated three more times around the part.

19:43

So, we're going to make three copies at 90 degrees, giving us a total of four flats.

19:48

Here we can see 3, 90 showing us that it's duplicated.

19:51

So, we'll "Apply" and "Close".

19:54

Let's press View Normal to Face Plane to make sure that we're normal to one of the flats, which we are.

20:03

So, we'll create a new Profile Group.

20:06

We'll choose Tool Position-left.

20:11

First, we'll choose a tool, so we'll uncheck Roughing, and let's go to Select Tools and we'll press All Diameters to search for what tools we have in our library.

20:22

We'll select the three-eighths End Mill.

20:32

Since we have a solid model, we can use the solid to give us the X_Surf and X_Depth.

20:38

So, let's go ahead and move this window to the top left of our screen and we'll take our model and rotate it just a bit.

20:45

So, we'll press Extract Parameters from Solid.

20:48

I'll go ahead and grab this sidewall here, which gives us both the X_Surf and the X_Depth and we'll press "Extract."

20:57

You can see we have an X_Surf of 0.160 and an X_Depth of 25 thousandths.

21:05

I'll name this Mill Flats and then we'll "Apply" and "Close".

21:16

To create our toolpath chain, we'll go ahead and select the Define Profile and Solid Model icon.

21:23

And select two points from the back of our flat.

21:27

We'll go ahead and verify that toolpath path using the Single Step icon.

21:32

Next, we'll go ahead and machine the cross holes on the 0.480 diameter of this part.

21:40

So, we'll open up our Setup dialog and we're going to create a new Face window for drilling.

21:45

So, we're going to select the Diameter Index Face Window.

21:50

This allows you to unwrap the geometry of the part, allowing you to draw holes around the diameter and drill them all at the same time.

22:07

Before we close the dialog, we need to set the OD to the OD that the cross holes are sitting on.

22:13

So, double clicking on the model, we can see the radius is 0.240, so we'll put the 0.480 diameter into OD.

22:21

And now we can "Apply" and "Close".

22:28

Since we have a solid model, we can do all of this from the solid, so we'll create a new Hole Group.

22:34

The first thing we'll do is Extract Parameters from the Solid.

22:40

So, we'll select the inside of one of the holes and press "Extract".

22:45

And we already have a cycle in here, but let's go through adding a new cycle.

22:50

So, we have the drill in here, but let's insert an operation so that we can put the Spot Drill and the Hole Canned Cycle-Spot Face in there as well.

23:01

We'll delete anything in hole diameter for spot drills so we can search for all spot drills.

23:07

We have a quarter inch diameter spot drill and we'll select our cross drill as well.

23:12

The Chamfer size, X_Surf, and Nominal Depth have been determined from the model itself.

23:18

So, we can go ahead and "Apply" and close this dialog.

23:23

The last thing we need to do is determine what holes on the model that we want to machine.

23:27

We could use the Single Hole on Solid Model icon to select one at a time or the Chain Holes on Solid Model icon, which selects holes that have the same diameter.

23:37

So, we'll go ahead and click on one and all of them are selected and then we can use our Single Step to verify our toolpath.

23:52

The last operation we have are the holes on the sub-side of the part.

23:57

So, we'll go ahead and open our Setup dialog and we're going to create a new Face window.

24:13

First of all, select Sub-Spindle and then we'll go into our Machining Functions and we're going to choose the Mill and Index machining function, which rotates C and keeps Y on Y0.

24:26

I'll go ahead and name that Drill Sub Holes and then we'll "Apply" and "Close".

24:37

Let's go ahead and open a new Hole Group.

24:48

And first, we're going to Extract Parameters from Solid to get the information from our holes.

24:52

So, I'll press the inside wall of our hole and we'll press "Extract".

24:56

Now, again, we already have a cycle created for this, but we'll go ahead and add a new cycle.

25:01

We'll go ahead and insert an operation for our spot drill, pick Spot Face as our canned cycle, and we'll delete the number in hole diameter so we can search for all spot drills.

25:14

Let's press "Select Tools" and we have a spot drill called Spot Drill Sub that's on our backworking slide.

25:20

Let's go ahead and select that one and we'll pick our drill that is also on the backworking side.

25:27

I'll change the hole diameter in spot drill to 0.0625 to match the drill.

25:33

And then we'll "Apply" and hit "OK".

25:36

And all of our information's already in there, Chamfer size, Z_Surf, as well as our Depth, so we can press "Apply" and "Close".

25:45

And last thing to do is just to select the holes off of the model that we want to machine.

25:50

So, let's choose the Chain Holes on Solid Model icon.

25:56

We'll select one of them and all of the holes are selected.

25:59

Well, then single step through this on our solid model.

26:13

Now, we're ready to go to our Process Table.

26:16

Let's press "OK" and first thing is to order our operations.

26:22

So, we'll start with facing the part, we'll then drill the ID and bore it out.

26:28

We'll turn, groove, thread, and then after our threading, we want to do our slot milling, so we'll move that up.

26:36

After that, we're turning the rest of the OD, milling the flats, cross drilling, and then we have our cutoff last in the Process Table.

26:46

If we look at our Time Chart, we don't have the main and sub-spindles synchronized right now.

26:53

Now, we're going to have to start synchronization under our end-working processes.

26:57

That's because the end-working tools are attached to the sub-spindle and those cannot be synchronized with sub-spindle processes.

27:03

So, starting from the first one below that, we'll open the Mode Switch.

27:11

Main spindle mode's Machining with One Tool and Sub Spindle-Machining with One Tool, and then we'll modify for all consecutive processes and we'll press "OK".

27:24

We'll then go to our first Sub-spindle process and do the same thing.

27:28

Main Spindle Mode-Machining with One Tool, Sub Spindle Mode-Machining with One Tool and modify for all.

27:33

Press "OK".

27:35

And then the last thing is on our Cutoff process, setting our pickoff.

27:40

Sub Spindle Mode follow support and we'll set a Z Support coordinate of 1 inch.

27:51

Now, we can press "Synchronize".

27:53

We can see in the Time Chart that our main and sub-spindle have now been synchronized together.

28:02

And we can simulate.

28:26

Once we're done simulating, we can view a finished part.

28:32

And we're ready to generate code.

28:34

So, we'll go to the Job Optimizer.

28:36

Let's go ahead and load a post file with our "Post Config File =?" button.

28:42

I'm going to select the Demo Post and then we're going to go back to Job Optimizer and generate an NC Program.

28:56

I'll press "OK".

28:59

We'll save that file.

29:03

And PartMaker shows us our generated NC Program.