Dowel Pin 2D (9:32 min)

00:06

In this lesson, we will learn how to get started with PartMaker.

00:10

First, a brief overview of the software, then how to set up our defaults and preferences, and finally, we will program and postcode for a simple dowel pin.

00:21

First, I'm going to open the Tools File.

00:24

This can hold tools for an individual job, one machine or many machines.

00:34

Next, we will open the Cycles File.

00:38

This contains repeatable homemaking processes.

00:44

We'll select a Material File from PartMaker's premade material library to help preset some feeds and speeds.

00:54

Lastly, we'll save our Job File to the same folder location as our Tools File and our Cycles File.

01:03

To access and make changes to our Tools, Cycles, and Material File, you will go to the ToolMinder and select from which one you would like to modify.

01:13

Before we get started with programming, let's take a brief look at PartMaker's interface.

01:18

The CAD/CAM Switch allows us to flip back and forth from a drawing mode to a toolpath creation mode.

01:25

Depending on which side of the CAD/CAM window you are on, you will see different icons on the side and top toolbars.

01:32

Next, we'll take a look at the Setup dialog, which describes the material size, guide bushing size, tool change positions, and it's where we create new face windows which define where we are on the machine and what we are doing.

01:48

Face windows are preset workplanes that control tool orientation and code output.

01:55

To set defaults within PartMaker, go to "Job Optimizer" and choose "Default".

02:00

First, we'll start with the turning defaults.

02:05

The following defaults have been preset to the recommended defaults.

02:09

It is important to set these before programming as some cannot be changed after programming has begun.

02:17

Next, we'll select Job Optimizer, Defaults, Milling.

02:22

These settings have also been preset to the recommended defaults.

02:28

To change preferences such as units and background color, we go to View, Preferences.

02:38

Now, we will get started with programming a simple dowel pin.

02:41

From the print, we can see that the pin has a half inch diameter, a 1.5 inch length, and 20 thousandths chamfers on either side of the front and back of the part.

02:51

Step one is going to be opening the Setup dialog and setting the stock material size.

02:56

We'll set the length to the final part length, which is 1.5 inches.

03:01

We'll set the OD to the stock material size, in this case, we'll use five-eighths stock.

03:09

The excess stock is the amount of material we want to face off the front of the bar.

03:13

For that, we'll set it to 15 thousandths.

03:17

The guide bushing length is going to be the landing size of the guide bushing.

03:21

Here, we'll do 750 and the guide bushing diameter is a value that just needs to be larger than the OD, so here we'll do 1 inch.

03:30

On the right hand side of the screen, we can see that there's only one face window in our list of face windows.

03:35

This must always start with the Main Spindle turn Face Window.

03:39

Now, let's close the Setup dialog and go to the CAD window with our CAD/CAM Switch.

03:44

To get started with drawing, we'll select the Connected Lines icon.

03:48

In the bottom of the screen, we can now enter coordinates.

03:52

Our first coordinate will be (0,0).

03:54

Using the Tab key, you can move from one to the other and then we'll press "Enter" to apply the coordinate.

03:59

The second coordinate will be X, 0.5, which we can type in the diameter due to the diameter programming setting in turning Defaults, we'll then go to Z, 1.5, and back down to X, 0.

04:17

Now, we can use the Chamfer icon.

04:23

We'll type in our chamfer size of 20 thousandths and we'll click on each corner of the part to apply the chamfer.

04:33

Now, we can mirror the part over the Z axis.

04:37

We'll click and drag a box over the part.

04:42

We'll select the "Mirror" button.

04:46

We'll select Multiple copies, Horizontal, and we'll press "Mirror" and "Close".

04:55

We'll flip back to the CAM side and from part features, we will select a New Profile Group to face the material off.

05:04

From our Strategy, we'll go with contouring.

05:07

For Tool Location, we'll select Face.

05:11

We'll uncheck Roughing and select a tool which will go with the 80 degree right handed tool and press "Select".

05:19

And then we'll name the group "Face".

05:24

Now, we can verify our toolpath by selecting the "Verify Work Group Toolpath" button.

05:30

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

05:35

After verifying, we can press the "Hide Every Toolpath" button.

05:39

Now, to turn the OD, we'll go back to part features New Profile Group.

05:44

We'll go with the contouring strategy again, but Tool Location-Out and Tool Orientation-Right this time.

05:50

Again, we'll uncheck Roughing and we'll select the 80 degree OD turning tool.

06:00

We'll then name the group "OD Turn" and then will "Apply" and "Close".

06:09

To chain our toolpath, we'll select the "Define Profile" icon and from our Snap Mode's toolbar, we'll choose the End of an Element Snap Mode.

06:19

We'll select the following points and then press the "Escape" key on the keyboard to exit the Toolpath Chaining Mode.

06:26

Again, we'll do a 2D verification of our toolpath.

06:32

And after verifying, press the "Hide Every Toolpath" button to get rid of our verification.

06:38

Now, we're ready to create the Cutoff operations.

06:40

So, part features, New Profile Group again and we'll go to Strategy and choose the Cutoff strategy.

06:49

Under Chamfer, we'll put in 20 thousandths, start X Point as radial, so we'll put a quarter inch.

07:00

We'll then select our Tool, where we'll choose the Cutoff Tool.

07:07

And we'll select the optimum path 1-2-1, which cuts to the bottom of the chamfer, lifts back up, chamfers, and then fully cuts the part off.

07:17

Now, we can give this a group name of "Cutoff" and "Apply" and "Close".

07:24

And then we will verify the toolpath.

07:27

Now, that we've completed programming, we can open the process table to order our processes, set our pickoff, and change any feeds and speeds we'd like to change.

07:36

To get to the process table, we'll go to Job Optimizer, Generate Process Table, and press "OK".

07:44

Once we're in the Process Table, if we'd like to reorder processes, we can simply click and drag those processes around.

07:53

To set our pickoff, we'll go to the mode switch, which is on the right side of the Cutoff Operation.

08:06

If we select Sub-Spindle Mode-Follow Support and set a Z support coordinate of 1 inch, that will pick the part off 1 inch from Z0.

08:19

If we want to change any feeds and speeds, we can double click on any of the processes.

08:24

Before posting code, we will do a 3D simulation.

08:27

Press the "Simulation" button and we'll press "Play" to view the simulation.

08:41

After simulating, we can press "Show Finished Part" to view and inspect our finished part.

08:48

To postcode, we need to load our post processor.

08:51

To do that, we'll go to Job Optimizer, "Post Config File=?" and select our post processor.

08:57

Note that this is made up of a main spindle and sub spindle posts.

09:00

Next, we'll go back to the Job Optimizer and select "Generate NC Program".

09:06

The Post Options dialog will appear, allowing you to put in your program number, by load subprogram number and also minimum and maximum spindle speeds.

09:16

From there we'll press "OK", name and save the file.

09:20

And once saved, PartMaker will show you your NC program.