Tutorial Lathe - Piston Part 1

IN THIS ARTICLE

1 - Overview

This tutorial cover the creation of the piston component below.

It will be used metric system to define coordinates and values.

At the bottom of this page , you can find all the related article for the concepts used in this tutorial.

In the specific article you can find more information about the software. As always, if something is not clear or missing , send me a message with the contact form so i can integrate the documentation.

The part will be created with 2 phases. Every phase will need a different setup item.

Here you can download project file created in this part of tutorial.

2- Add First Setup

At first , we need to define the first setup . We choose a Lathe Setup since we are going to do some turning operations to the part.

The setup will be like the parent folder of all the operations related to current stage

So from the main page you can click on [Lathe Part] button in the left column 

or

from Menu -> Lathe -> New Setup : Lathe 2 Axis

At this point you will get this screen. Here you can edit property at setup level like the machine type and machine definition to use.

Of course , you can change any of this values later, by clicking on setup item in treeview.

In this screen you can edit selected origin, program name, program number, lathe spindle limiter and all the necessary parameters related to setup.

See here for more detailed info on setup screen.

For this tutorial, set this properties :

Description -> Piston Setup 1

Origin -> WCS 1

Program Name -> Custom Piston

Program Number -> 50

Spindle Rev. Limit -> 1500

Leave other properties with default values

Press [OK] to proceed to next step.


3 - Stock Definition

More info on related page .

For this tutorial, set this properties :

Stock Type -> Cylinder

Selected Material -> Mild Steel

Outer Diameter -> 100

Length -> 105

Ref. Coo Z -> 2.5

Press [OK] to proceed with next step.


4 - Face Turning

Here more info on face turning.

As usual, the first operation to add in a lathe component part is the face turning.

From Menu -> LATHE -> Face Turning

Edit these fields :

Material to remove : 4.5 . This distance is measuered from Reference Z value in Z + direction. That means the toolpath need to consider 4.5mm of material to remove.

Finish Allowance : 0.1 . It's the allowance material left by the roughing operation to finish tool.

Enable the finishing operation


5 - External Turning

From Menu -> Lathe -> External Turning -> Step Profile

For this profile , is enough one diameter . In step profile grid control, edit in this way :

Diameter : 93.2

Depth : 100 - 26 , the calculator will solve to 74 . 

Sometimes in part drawing there isn't direct indication of the quote you need.

But you can find out with some simple calculation. With the integrate calculator , it's enough input your string into numeric fields and get the value.

Init Chamfer : 2x20 . With this you can draw a chamfer of 2 mm width and an angle of 20° . If you insert just ' 2 ' you get the common angle at 45°

Press [OK] to accept the profile. You can edit this profile later. To open up again this step profile edit screen you can :

- Right Click on viewport onto the profile and click on EDIT from the context menu.

- Click on edit button in geometry list in work screen.

In external turning edit screen set :

Finishing Allowance X : 0.25

Finishing Allowance Z : 0.1

Enable finishing operation

Press [OK] to save and return to home view


6 - Central Drilling

Now you need to work the internal part of the component.

First you need to add a drill operation , from MENU -> LATHE -> Lathe Central Drilling

The closest insert drill available in my tool store is 24mm diameter , so under the drill operation , set :

Diameter : 24

Depth : 24 * 3 , Usually an insert drill have an max working depth of 3 x Diameter . In the field you can see 72 mm.


7 - Edit Tool

Probably the auto select tool for the drilling operation is a 24 HSS drill. I need to edit it and select a insert drill.

Click on Select Tool Field to open tool selection dialog.

This will open the tool selection dialog.

Select the 24 mm drill and edit the tool geometry property as below :

Length: 24*3

Total Length : 120

Tool Geometry Type : Flat 180°

And then the cut data as below. Take this value as indication . You need to use cutting data indicated from your tool builder related to the stock material .

Cutting Speed : 150

Fz : 0.14

Drilling Mode : Direct

Click on [Select Tool] button in the bottom part of tool selection window to save and return to the main window.

Here you can click [OK] to close the drilling operation screen.


8 - Internal turning

From MENU -> Lathe -> Internal Turning -> Step Profile

This operation is very similar to the previous external operation.

Insert this values in step profile pattern:

Diameter : 28

Depth : 58

Init Chamfer : 3 

Press [OK] to close the profile pattern screen and press [OK] again to close the internal operation screen.


9 - Internal Threading

From Menu -> Lathe -> Internal Threading

This part require a M30x2 thread, so set: 

Select thread category : Metric

Select Thread : M30 x 2

Lenght : 56

All the other fields get filled by itself when you define the [Select Thread] property.

If the thread you need to do it's not available or you need to change something in default thread property, use the thread table. See the related article for more info.


10 - External Grooving

From Menu -> Lathe -> External Grooving -> Standard

For the first groove geometry , set :

Outer Diameter : 93.2

Inner Diameter : 88.87

Groove Width : 15.0

Start Z : -52.0

External Chamfer : 0.25

If you need create more groove geometries, you don't have to add additional machining operation.

Just add a new shape to geometry list.

Add -> Standard

For this second groove geometry set:

Outer Diameter : 93.2

Inner Diameter : 78.5

Groove Width : 6.4

Start Z : -33.6

External Chamfer : 0.25

Internal Chamfer : 1.0

Corner Mode ( related to internal chamfer ): Fillet  

For the third and fourth groove, proceed to add another standard geometry to the list and use the same parameter of the second groove.

Just change the Start Z value, as -20.4 for the third and to -7 for the fourth groove geometry.

Return in the grooving operation screen. 

Under roughing operation set: 

Finishing Allowance X  : 0.15

Finishing Allowance Z  : 0.15

Enable finishing operation.

Press [OK] to return to home.


At this point you should have something like this.

The second part of this tutorial will cover the completation of piston part.

Still need help? Contact Us Contact Us