Advanced Turn Mill, 5-Axis, and 3D Surfacing (23:51 min)

00:12

To get started, we'll go ahead and import a solid model.

00:15

So, we go to File, Import, X_T Parasolid, and we'll choose our model and press "Open".

00:28

When programming off of a solid model, the first step is always to set the part origin.

00:33

So, we'll go to Edit Part Coordinate System, press "Set Part Origin" and from our dropdown, we'll choose Face Center as our selection method.

00:45

I'll press the front face of our part, press "Set" and we'll press View Normal to Face plane, making sure that our Z axis is facing in the horizontal direction and our part is on the left of our origin and we'll press "Close".

01:02

The next step in programming our model will be to take a section of the part.

01:06

We'll use the Extract Turn Geometry icon and take a look at the turning plane angle that we're using.

01:12

Forty five degrees looks to go through the correct section of the part, so we'll press "OK".

01:18

Then we'll convert curved edges to arcs so that we can get G2 and G3 arcs in our code.

01:25

Let's open up the Setup dialog and see what length and OD that the software found from the model.

01:31

So, it looks like 3 inches in length, 3 inches in diameter.

01:37

We'll set the Axis Stock to 15 thousandths here so that we can face off 15 thousandths from the front of the part.

01:44

And we'll set the Work Shift or how far we're sticking out of the chuck to 4 inches.

01:50

We're first starting with a Main Spindle-Turning Face window and we'll press "Apply" and "Close".

01:57

Let's now go to our 2D side and we'll open up a new Profile Group in order to do our facing operation.

02:06

From the strategy, we'll select Contouring and Tool Location face.

02:12

I'll uncheck Roughing and will select a tool.

02:15

I'll choose this 55 degree OD Turning Tool, which is number one on our tool head.

02:21

And then we'll name that "Face" and "Apply" and "Close".

02:25

PartMaker generates the toolpath automatically when you choose a facing operation, and then all we need to do now is verify the toolpath, so we'll press "Verify Work Group Toolpath".

02:37

We'll show the tools Hollow and we'll verify with the Delay of about a 3.

02:44

That looks good.

02:45

So, now we can clear our verification with the Hide Every Toolpath icon and we'll move on to our next operation.

02:53

Before that, I'll select another color and we'll go ahead now and turn the OD.

02:58

I'll choose a new Profile Group.

03:01

Since we have a good amount of roughing to do on this part, we'll choose the Turning Strategy.

03:06

Tool Location-Out and Orientation-Right, and I'm going to define my Cutting Limits by Part Profile Boundaries so that they follow the toolpath that I draw instead of the stock boundaries.

03:18

Let's check finishing so that we can do both roughing and finishing on this part.

03:22

We'll select Tools, choosing the OD Turn 55 for both rough and finish.

03:29

I'll leave 10 thousandths in X and 10 thousandths in Z for our finishing tool and I'll change my Depth of Cut to 50 thousandths per pass.

03:40

And I'll name this "OD Turn" and "Apply" and "Close".

03:47

Now, let's press the Define Profile icon with End of an Element Snap Mode to generate our toolpath profile.

03:53

I'll start here and go to here.

03:57

Then I want to cross over this groove, so I'll use the horizontal constraint and then we'll click up to the back of the part.

04:06

And now I'm going to switch to ZX Coordinates Snap Mode.

04:10

And in the X direction, I'm going to say @, which is incremental and move up 10 thousandths and that's going to force the tool to go there, even though there is no material on top of our stock material that we need to take away, since that is the 3-inch diameter.

04:27

We'll go ahead and verify that toolpath.

04:46

Now, let's move on to the grooving operation.

04:49

Again, we'll choose a new color.

04:51

I'll choose a Profile Group, and from our Strategy-Grooving, Tool Location is Out since this is an OD groove and we'll select a Tool.

05:01

In here, we have a 125 with grooving tool, so we'll select that and I'm going to name this "OD Groove" and "Apply" and "Close".

05:14

Let's pick the Define Profile icon and the End of an Element Snap Mode and outline the groove and then will verify.

05:28

For our last turning operation on the main spindle, we'll create our cut off.

05:34

So, let's go to new Profile Group, from Strategy, we'll choose Cut Off.

05:40

I'll select the tool choosing the cut off tool that we have is number 9 on our tool head.

05:48

I'm going to name this cut off and then we need to make sure that we have our distance is set correctly, so we have 3 inches from the face of the part, that's where we want our cut off to be.

05:59

Let's add a Chamfer to that, we'll do 10 thousandths chamfer.

06:03

Start X Point as a radio value and since our finished part is going to be 3 inches, we do want this to be 1.5, and then I'll press Optional Path 1-2-1, which is going to cut down to the bottom of the chamfer, lift up, and then chamfer, and cut the rest of the way off.

06:22

Let's "Apply" and "Close".

06:23

And PartMaker generates that toolpath for us and we can verify.

06:33

Now, let's move on to the milling operations of our part.

06:37

We have four holes, four slots, and a pocket in the center of the face.

06:43

So, the first thing to do is go to our Setup dialog and we'll create a new Face window.

06:48

And for our four holes and slots around the part, we're going to choose the Mill End Index face window.

06:57

Let's "Close".

06:60

And we'll start with our drilling operation.

07:01

Let's create a new hole group and we'll use Extract Parameters from Solid to gather information from the model.

07:08

I'll press the inside of one of the holes, press "Extract" and we have a cycle already created with the Center and Drill.

07:15

So, we'll press "Select".

07:19

Now, what we need to do is select the location of those holes from the model and we can do so with the Chain Holes on Solid Model icon.

07:27

So, we'll select one and the rest of these similar diameters will be selected and then we can go ahead and step through this on our solid model.

07:41

Now, we're going to mill the slots.

07:45

So, before we do that, let's go ahead and double click on the face and transfer planar geometry so that we have that geometry up in our 2D window.

07:54

We'll create a new Profile Group.

07:58

I'm going to go straight to "Finish" and let's "Select Tools" and choose all diameters.

08:03

So, we have a one-eighth end mill facing in the Z direction, let's press Select on that, and we'll move this to the top left of our screen and bring our model back up so that we can extract parameters from the solid, we'll extract parameters from the solid by selecting the checkbox.

08:21

We'll press the sidewall so that we get the front of the feature as well as the back and we'll press "Extract".

08:28

For Axial Step, let's put it at 50 thousandths for how far we step back in Z each pass and we'll call this "Mill Slot" and "Apply" and "Close".

08:39

Now, we need our toolpath itself and we'll do so in the 2D, so we'll grab the Define Profile icon, I'll select the Circle Center snap mode, selecting this as our center.

08:53

I'll grab the Screen snap mode and a vertical constraint and we'll just pull a line all the way out of the part to make sure that the tool clears.

09:04

And then I'll click on that profile and let's go ahead and reverse that to make sure that the tool starts on the outside, working its way in.

09:11

The next step is to take that toolpath and we'll go to Edit, Transform, Rotate, and we're going to rotate this with multiple copies.

09:20

Three copies around the part at 90 degrees and rotate.

09:27

And now, we can verify.

09:30

And we can do this on our solid model as well.

09:36

Now, let's move on to the pocket on the front of the part.

09:39

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

09:44

And for this one, if we want continuous Z axis motion with Y at Y0, we'll choose Mill End Polar.

09:53

And I'm going to name it End Polar and we'll "Apply" and "Close".

09:57

Again, we'll take the geometry from the front of the part, double click on it and transfer it up to our 2D window so that we have a profile to select.

10:09

We'll open a new Profile Group.

10:11

From Strategy, I'll choose Pocket Mill.

10:15

We're going to go straight to finish on this Pocket, so we'll uncheck Roughing.

10:21

I'll select Tools and press "All Diameters" to see all of the tool options that we have.

10:26

We have a one-eighth End Mill in the Z axis, I'll select that one.

10:32

Let's move this window to the top left of our screen, so that we can grab geometry from our part.

10:39

I'll press "Extract Parameters from Solid", select a sidewall and press "Extract", that gives us our surface and our depth.

10:49

And then I can name this "Pocket".

10:52

And lastly, let's choose an axial step, how far we wanted to step in in Z each time, so let's say 50 thousandths in Z and we'll "Apply" and "Close".

11:04

Lastly, we need to select an outline of the pocket, so we'll use our Change Geometry icon and select the pocket in the 2D.

11:15

Let's watch that on our solid model.

11:29

Now, let's move on to our 5-axis work.

11:34

We'll go to the Setup dialog, create a new face window and we'll choose a Mill 5-Axis Plane to get started.

11:42

So, we'll call this "5-axis 1" and for the other side of the part, we'll end up creating another 5-axis face plane.

11:50

So, starting with this feature right here, we'll select the face or press "Define Face Plane" that sets our B and C angle as well as our local origin, and we'll press "OK" and View Normal to Face Plane.

12:06

Now, we can take this face right here, double click on it and Transfer Planar Geometry as Curved Adjust to Arcs up into our 2D window, and the first operation that we'll do is flatten off this face.

12:21

So, I'll select a new Profile Group.

12:24

We'll use that Contour Mill Strategy and do Tool Position-Left.

12:30

I'll move this window to the top left of our screen.

12:36

And let's just make sure that using Extract Parameters from Solid, that we have the correct surface in depth.

12:41

So we'll set that to this surface here, press "Extract", and we still have zero and zero, and that's because our face plane is actually set on that surface.

12:52

We'll press Select Tools, and I'm going to choose the quarter inch Z tool and we're going to leave it on Roughing so that we can rough in the radial direction.

13:06

We'll set our Axial Step, how far do we want it to take per pass in the X direction, we'll press 0 and that's going to do one pass full depth.

13:21

We'll set the Initial Stock, so how much material do we have on the right or left side of the line that we draw, so we'll put 1.5 inches.

13:31

And then lastly, let's go to our Leads and we'll zero out the arc radius and angle, and we'll extend the line length.

13:38

So, it's going to go on a straight line before and after our toolpath by half inch, and we'll copy that to our Lead Out and press "OK".

13:48

So, let's name this "5-Axis flat 1" and we'll "Apply" and "Close".

13:55

The last thing that we need to do is create the toolpath itself.

13:58

So, we'll use the Define Profile icon and click from here to here.

14:03

And let's verify that toolpath.

14:06

So, because of the initial stock being 1.5 inches, we started all the way over to the right and we're roughing towards the line that we drew.

14:16

The next operation that we're going to do is rough out this pocket using a 3D strategy.

14:23

So, we'll start a new Surface Group.

14:26

We'll do roughing and we're going to choose that same quarter inch End Mill.

14:33

In our options, we'll select the Style, so I'm going to go with an Offset All style, which is going to offset the shape of the profile that we're cutting as well as the stock material.

14:47

We'll set our Cut direction to both climb and conventional.

14:51

We'll leave 10 thousandths on the finish surface , and we'll set our stepover to 100 thousandths, and stepdown, we'll leave it at 50 thousandths.

15:02

The last thing that we need to do in this dialog, we're going to go to Limit and we're going to set a maximum limit of zero.

15:10

So, zero is located at our face plane, which is on the flat surface right now.

15:15

And we don't want the roughing strategy to start above that and rough out our stock material, because it's already gone from the last operation we did, so we'll set a Z limit.

15:27

We'll call this "Rough side 1".

15:33

"Apply" and "Close".

15:35

And using the 2D side and the Change Geometry icon, we'll enclose that pocket and we'll verify it on our solid model.

15:50

Now, that it's roughed out, we need to go ahead and finish this pocket.

15:57

So, we'll grab another Surface Group.

15:60

I'll uncheck Roughing, goes to Finish.

16:04

Under Select Tools, I'm going to choose this quarter inch ball mill.

16:10

From the Strategy, raster finish is back and forth, but we're actually going to choose 3D Offset Finish, which will follow the contours of the model.

16:19

Under Options, I'll set my Stepover, so we'll go with 25 thousandths and we're going to do a climbing direction.

16:27

So, we'll call this Finish Pocket.

16:33

"Apply" and "Close".

16:35

And again, we're going to enclose the pocket with a profile.

16:47

Now, we're ready to machine the other side of the part.

16:50

So again, because it's on a different B and C angle, we'll go to the Setup dialog, create a new face Window.

16:58

It's still going to be a Mill 5 Axis Plane, but we'll call this one 5-axis 2.

17:06

We'll grab this face and press "Define Face Plane", press "OK" and View Normal to that face plane.

17:15

Now, we'll do the same thing that we did last time, we're going to double click on this face, transfer the Geometry to arcs.

17:22

So, we see it up in our 2D window.

17:27

I'll press new Profile Group, choosing a contour mill with tool position left, and we'll choose roughing again because we're roughing in the radial direction.

17:38

We'll choose the same quarter inch End Mill.

17:43

Z_Surf and Z_Depth should still be 0 because we set the face plane 2 there.

17:50

We'll set our Axial Step to 0 again, 1.5 inches of Initial Stock.

17:56

And under our Leads, we'll do the same thing, zero out the Arc Radius to a half inch Line Length and 0 Angle and copy that to our Lead Out.

18:05

And then I'm going to name this group "5-axis flat 2" and "Apply" and "Close".

18:13

And we'll draw our profile using the Define Profile icon and End of an Element snap mode and verify.

18:29

Now, we need to drill these holes, so we'll select a new Hole Group.

18:34

We'll extract parameters from the solid and I'll grab the inside of one of the holes and press "Extract".

18:40

Now, we already have a spot drill and drill operation for this 375 drill, so we'll press "Select", it grabs the Z_Surf as well as the Depth.

18:53

Now, looks like our spot drill did not grab a depth, so let's uncheck Extract Parameters from Solid and we'll put a small five thousandths chamfer on this hole.

19:04

And then when I press "Apply", you'll see depth has updated.

19:10

And we'll press "Close".

19:12

The last thing is to use the Chain Holes on Solid Model icon to tell it where those holes are located, so I'll click on one, both are selected.

19:23

Then we can single step to see this operation.

19:29

For our last operation, we'll go ahead and move this radio slot around our part.

19:35

So, first, we'll go to the Setup dialog, we'll press "New" and we're going to select the Mill Cylinder Face window.

19:45

I'll name this "Mill Cylinder".

19:48

And first, we need to check what our OD needs to be for this particular face window.

19:54

So, we'll double click on the outside of our model, radius is 1.5, so 3 inches will be OK for our OD, we just want that to match whatever the turn diameter of the section that you're about to mill.

20:07

So, let's "Apply" and "Close".

20:11

I'll double click on the bottom surface of the slot and we'll transfer Unwrapped Geometry to arcs.

20:21

Now, we can create our toolpath, so we'll go to a new Profile Group.

20:28

We're going to do an on-center contour milling strategy.

20:33

We'll select a tool.

20:36

We'll go ahead and choose all diameters and we'll pick this one eighth diameter X oriented end mill.

20:45

We're going to go straight to Finish, so I'll uncheck Roughing.

20:49

And then we need to set the X surface and depth, so we'll click "Extract Parameters from Solid", we'll select the sidewall and press "Extract".

20:59

The last thing to do is to set our Axial Step, how much we want to take in the X direction per pass and we'll set that to 50 thousandths.

21:18

Now, our last step in this is to actually change the toolpath.

21:23

So, we will use the Define Profile icon, I'll use the Circle Center Snap Mode and we're going to click around this rectangle.

21:35

And then we can verify that toolpath.

21:46

Now, that we've completed all of our operations, we can go to the Process Table.

22:01

In our Process Table, we can go ahead and reorder anything that we want to reorder.

22:06

So, I'm going to line up the 5-Axis Flat 1 and Flat 2 just by clicking and dragging.

22:13

And then everything else in here looks to be in order.

22:18

We also need to set the pickoff during our cutoff operation.

22:22

So, I'm going to go to the mode switch on our cutoff line.

22:26

We'll set part support and we'll give it a coordinate that we want to grab onto.

22:30

So, we'll say 1 inch onto the part.

22:33

Lastly, we'll set the Eject to this last operation because there are no sub-spindle operations on this part.

22:41

Now, we can go to simulation.

22:48

We'll select Simulation Options to slow our simulation down and we'll set the Time Delay to 1 and we'll play.

23:08

After completing the simulation, we can run through a finished part.

23:23

And now we're ready to postcode.

23:25

We'll go to the Job Optimizer and we'll select a Post file.

23:30

I'm just going to use this sample file.

23:35

And then we'll go to Job Optimizer, generate NC program, and we'll save that file.