Learning Pro/Manufacturing Using Pro/Creo Elements

iUniverse, Inc.

Contents

Tutorial 1 (3 Axis Milling - Engraving)................................................6Tutorial 2 (3 Axis Milling - Face Milling).............................................29Tutorial 3 (3 Axis Milling - Volume Rough and Profile Milling).........................47Tutorial 4 (3 Axis Milling - Volume Rough and Surface Milling).........................76Tutorial 5 (3 Axis Milling - Volume Rough and Drilling Cycle)..........................100Tutorial 6 (3 Axis Milling - Volume Rough, Drilling and Tap Cycle).....................127Tutorial 7 (3 Axis Milling - Volume Rough and Threading Cycle).........................165Tutorial 8 (4 Axis Milling - Volume Rough, Drilling and Engraving).....................200Tutorial 9 (5 Axis Milling - Surface Milling)..........................................256Tutorial 10 (5 Axis Milling - Surface and Profile Milling).............................289Tutorial 11 (2 1/2 Axis Milling - Expert Machinist)....................................327Tutorial 12 (2 Axis Turning - Area Turning)............................................374Tutorial 13 (2 Axis Turning - Area, Profile, Groove and Thread)........................399Tutorial 14 (2 Axis Turning - Area, Drilling and Boring)...............................434Tutorial 15 (Milling and Turning)......................................................464Tutorial 16 (2 Axis Wire EDM)..........................................................492Tutorial 17 (Creating Post Processors).................................................507

Chapter One

Engraving is used when tool follows a specified trajectory. Some key feature covered in lesson are mentioned below.

? Program zero (Machine coordinate) is created

? Tool is added to the list

? Parameters (feed, spindle speed, etc) are defined

? CL (Cutter location) data and G codes are obtained for a machine

Create a new part file

Type in the name and make sure Part radio button is selected and Select OK

Select Extrude

Go to Placement and Select Define to Select sketching plane

Select Top Datum plane as sketching plane and Right Datum as Orientation Right

Select 2 point centerline and create Horizontal and Vertical centerlines

Select Rectangle

Draw a rectangle of 5.5 by 3.5 as shown

Select check mark to confirm

Give thickness of 0.75 and then check mark to confirm

Select Sketch Pick the Top surface of part as sketching plane and Right Datum plane as orientation Right

Select the Text icon Left click on part face and then left click above it to give height of text

Type in CAM and make sure to change the Font to Cal_alf and press OK

Save the part

Change the dimensions and check mark

Create a new file for manufacturing

Type in the name and make sure Manufacturing radio button is selected and Select OK

Use any of these icons to bring the work-piece in

Or

Select the part and press Open

Part needs to be oriented with ASM Datum planes. Right click on background and select Default Constraint and press Check mark.

Or

Select Default from pull down menu and check mark

(if you choose the drop down menu from insert , select same model in the box)

The reference part has been assembled and for this tutorial no Stock (work-piece) is required because reference part has the same dimensions as stock (Stock will be created in later tutorials).

A co-ordinate system will be created on reference part with respect to which all the machine co-ordinates will be obtained (known as program Zero). The orientation of program zero for 3 axis mill is shown on right

To create Program Zero (Coordinate System) Select Coordinate system

To create the co-ordinate system, select surfaces by holding Ctrl key in the order shown.

This is not correct orientation of Coordinate system in default orientation (Press Ctrl-D together) or

Select Orientation tab to correct the orientation

Z is normal to above surface

X is normal to above surface, But X is positive towards Right so Flip the direction

When the orientation of Co-ordinate system is correct.

Positive X is pointing towards Right, positive Y is pointing above and positive Z is out of reference part. Select OK A new Cooridnate system will be created ACS0

Now, setup the machine for milling process.

Click on this icon to Select type of machine and process (Milling, Lathe ,etc)

Machine type: Mill

Number of Axis: 3

Select OK to confirm the selection of machine

Click on this icon to Select Program Zero (that is the reference coordinate for the part and everything is measured from there)

Select the coordinate system ACS0

Click on this icon to select Retract surface (the tool will move up to this surface after each machining process)

Select top surface of part and give an offset value of 0.5 for Retract plane. Select OK to confirm.

Press OK on Operation Setup box to confirm the changes made.

New Icons will appear and part is ready to be machined. These icons can also be accessed from Steps menu.

Tools can be created now or in machining sequence. To create tool now select any of the two options listed below

or

Change Tool type to Grooving and diameter to 0.1 and Apply. If additional tools are needed, select File >> New Once required number of tools have been added select OK to exit

To select Engraving process. Click

Or

If this option is selected, program will ask to input Name for machining sequence

If this option is selected, program will ask to select a coordinate system for program Zero , otherwise it will by select the default one which is ACS0 .

When Start and End options are selected, tool move to this point before doing machining and when machining is done tool moves to an end point. Points can be created using point icon

Only Select Tool, Parameters and Datum Curve and Press Done.

The options that are selected, program will ask for more information when Done is pressed.

Select the tool 1 for machining operation and select OK

Speed tool moves in part

Material removed in each pass

Total groove depth

Spindle Speed

See below

When values have been changed, Press OK to confirm and exit

Clear Dist (Clearance distance) is the distance when tool starts to follow the feedrate command (G01), all tool motions before Clear dist are in rapid mode (G00) Make sure Clear Dist is less than the height of Retract plane (that was selected earlier and for this tutorial is 0.5).

Select the CAM sketch and Select Done/Return.

To see tool path, Select Play Path and Screen Play

To play the tool motion

To slow down the tool motion

Too motion

Screenplay only give tool motion. To see the material removal NC Check should be used. To access NC Check, one option needs to be activated

This process needs to be carried out anytime after Pro/Creo Elements is started

Select Tools >> Options

Type in nccheck_type in Option and nccheck in Value. Press Add/Change and Close the window

To see material removal, Select NC Check

Press Run to see the Material removal animation (Step size can be selected to slow down the animation)

Material Removal

If anything needs to be changed in machining seq. Right click on...