Figure 1: NC Lathe menu

Click To See: How to Use Online Documents SURFCAM Online Documents 685)&$0Ã5HIHUHQFHÃ0DQXDO 5 /$7+( 5.1 INTRODUCTION The lathe mode is used to perform operations on 2D geometry, turned on two axis lathes. SURFCAM is compatible with any lathe axis orientation. The axis orientation is user-configurable in SURFCAM but the actual axis orientation and direction can be overridden by the post processor. Standard output for a variety of manufacturers can be generated with the sample post processors supplied. Refer to the online SURFCAM Support Utilities Manual, Chapter 2: Post Processing Introduction and MPost starting on page 31 for the procedure for configuring the different post processors. For display purposes, all references to the tool orientation are based upon the turret being to the rear of the part. Front lathe machine code is produced by the post processor. You can generate NC programs in a local coordinate system. Thus you can machine different sections of the work with independent machining orientations a necessity with many parts. Turn Face Figure 1: NC Lathe menu Turn is used most often to machine the part along the length of the material with cutting moves parallel to the Z axis. It can, in fact, be used to cut at any angle to the Z axis in the correct circumstances. Refer to Section 5.2: Turn on page 321. Face is used most often to machine the part along the diameter of the material with cutting moves perpendicular to the Z axis. It can, in fact, be used to cut at any angle to the Z axis in certain circumstances. Refer to Section 5.3: Face on page 325. Face Off Face Off is used to remove material from the face of the part in preparation for performing other turning operations. Refer to Section 5.4: Face Off on page 328. Groove Refer to Section 5.5: Groove on page 330. Thread Thread is used to create inside or outside canned cycle threads. Refer to Section 5.6: Thread on page 332. Drill Partoff Options Drill is used to drill the face of the part. Only the part centerline can be drilled. Refer to Section 5.7: Drill on page 334. Partoff is used to cut a turned part off of the bar stock from which it was machined. Refer to Section 5.8: Partoff on page 337. Click Options to display a dialog box that contains all the NC mode Options tabs. Refer to Section 5.1.4: Lathe Options Tab on page 318. SURFCAM Reference Manual, Chapter 5 Lathe

296 SURFCAM Reference Manual, Chapter 5 Lathe Each operation has a separate dialog box which will be displayed after you have selected an operation and identified the geometry on which it will be performed. After you click OK on a Lathe dialog box, you will be prompted to pick a Retract and Clearance point. Retract-Clearance Points A lathe Retract Point is the point you want the tool path to begin and end. It will often be the point where you want tool changes to be made. A lathe Clearance Point defines a level or distance from the Z axis. The tool will rapid to and from this level (perpendicular to the Z axis) at the start and end of the lathe cycle, as it moves from and back to the Retract Point. Clearance points are most often used with ID operations. You can skip selecting a Retract Point or a Clearance Point by clicking Done on the Lathe menu. 5.1.1 Configure Lathe View SURFCAM provides different lathe coordinate systems. Click Options > Axis. Then select Mill Axis, Lathe Radius, or Lathe Diameter. Refer to Figure 2: Mill Axis, Lathe Radius and Lathe Diameter. VIEW 1 VIEW 7 WORLD DIALOG BOX MILL LATHE RADIUS

SURFCAM Reference Manual, Chapter 5 Lathe 297 LATHE DIAMETER Figure 2: Mill Axis, Lathe Radius and Lathe Diameter 5.1.2 Tool Information Tab. The Tool Information tabs for all lathe operations are the same except for the Drill tab, which has fewer parameters and two the others don t have. Figure 3: Lathe Turn Tool Information tab

298 SURFCAM Reference Manual, Chapter 5 Lathe For a description of the parameters not in the following list, refer to the SURFCAM Getting Started Manual, Chapter 3: Common NC Parameters, Section 3.2: Tool Information Tab on page 64. Tool The name of the currently selected lathe or lathe drill tool is displayed. The corresponding lathe tool reference number is displayed on the button. To select a different tool, edit a tool record or add a new tool click the button to display the Select Lathe Tool or Select Lathe Drill Tool dialog box. Refer to 1. Section 5.1.2.1: Select a Lathe Tool on page 299, 2. Section 5.1.2.3: Select a Lathe Drill Tool on page 307, 3. Section 5.1.2.2: Edit or Add a Lathe Tool on page 302, or 4. Section 5.1.2.4: Edit or Add a Lathe Drill Tool on page 311. Turret Define which turret to use when cutting the part. Five Turrets for holding tools are available on Mill/Turn machines: Rear, Front, Saddle, Main, and Rail. Z Gauge Length This is an arbitrary estimate of the distance, parallel to the Z axis, from the center of the turret to the tip of the tool. X Gauge Length This is an arbitrary estimate of the distance, parallel to the X axis, from the center of the turret to the tip of the tool. Spindle Speed (RPM) Specifies the spindle speed in either RPM (revolutions per minute) or CSS (constant surface speed) selectable in the third column. The direction of the spindle rotation can be set to clockwise (CW) or counterclockwise (CCW) in the second column. SURFCAM calculates Spindle Speed using the following formulas: Inches: Millimeters: Spindle Speed = (Surface Speed*12) / (3.14159*Diameter) Spindle Speed = (Surface Speed*1000) / (3.14159*Diameter) Surface Speed This is a value from the Material Library that is associated with the material being cut and the material from which the tool is made. Diameter This is the value, listed in the Tool Library, for the diameter of the tool being used. You can override this calculated value. Feed Rate Specifies the linear feed rate as inches/millimeters per revolution or inches/millimeters per minute, depending on which option IPR or IPM is selected from the second column.

SURFCAM Reference Manual, Chapter 5 Lathe 299 SURFCAM calculates Feed Rate using the following formulas: IPR Feed Rate = Chip Load per Flute*Number of Flutes*Chip Load Factor IPM Feed Rate = IPR Feed Rate * Spindle Speed Chip Load per Flute and Number of Flutes These are values from the Tool Library. Chip Load Factor This is a value from the Material Library associated with the material being cut and the material from which the tool is made. Spindle Speed is the previous parameter on this tab. You can override this calculated value. In the second column, select either Inches per Minute (IPM) or Inches per Revolution (IPR) [Millimeters per minute (MMPM) or Millimeters per Revolution (MMPR)]. The selection determines the Post output code for the Feed Rate. Note: Inverse time feed rates are calculated in the post processor based on the desired feed rate and the actual length of the move. When these feed rates are used, the NC code must have a feed rate programmed on each block. This is to maintain a constant feed rate, in inches per minute, across the part. Check the machine tool documentation for the feed rate type requirements. Plunge Rate Specifies the plunge rate in inches per minute or millimeters per minute depending on the selection made in the Main menu Options sub-menu. This is the rate at which the tool will feed if it is moving directly down at the beginning of a cutting cycle, or as it moves between passes in feed and bidirectional retrace modes. SURFCAM calculates Plunge Rate by dividing the initial calculation of Feed Rate by two. If the Feed Rate value is overridden, the Plunge Rate is not recalculated. You can, however, override the Plunge Rate value. In the second column, select either Inches per Minute (IPM) or Inches per Revolution (IPR) [Millimeters per minute (MMPM) or Millimeters per Revolution (MMPR)]. The selection determines the Post output code for the Plunge Rate. Nose Radius Nose Radius is a Tool Library value associated with the selected tool. 5.1.2.1 Select a Lathe Tool To select the tool to be used in a Lathe operation, click the button to the right of the tool description on the Tool Information tab. Figure 4: Tool parameter on Tool Information tab A Select Lathe Tool dialog box will be displayed. Refer to the SURFCAM Getting Started Manual, Chapter 3: Common NC Parameters, Section 3.2.1.1: Select Tool on page 70 for a description of the four uses of the Select Tool dialog box.

300 SURFCAM Reference Manual, Chapter 5 Lathe Figure 5: Select Lathe Tool dialog box Toolbar Use the toolbar to select a tool, add a new tool, or edit the features of an existing tool. Go to first record. Go to previous record. Go to next record. Go to last record. Choose a face/turn tool. Choose a round tool. Choose a lathe triangle tool. Choose a lathe thread tool. Choose a lathe groove tool. Add a lathe tool to the library. Edit / Save information in the library. Delete the current tool record. Figure 6: Toolbar buttons on the Select Lathe Tool dialog box Tables This box is available so you can select from different tool tables that you might have. Available Tools This list box will display available tools of the currently selected class of lathe tools Face/Turn, Round, Triangle, Thread, or Groove. The tool reference number and description appear in the list. Selecting a tool in the list selects its parameters

SURFCAM Reference Manual, Chapter 5 Lathe 301 for the next NC lathe operation. You can change any of these tool parameters in the text fields of this dialog box. Tool parameter changes affect only the current operation and are not saved in the lathe tool library. Lathe Tool Parameters The lathe tool parameters that can be changed are displayed next to the Available Tools list box. Face/Turn and Triangle Round Thread Figure 7: Lathe Tool Parameters Groove Nose Radius The radius of the nose of the tool.

302 SURFCAM Reference Manual, Chapter 5 Lathe Radius The radius of a round tool. Inscribed Circle The diameter of the largest circle that fits inside the tool outline. Groove Width This is the groove tool width. Back Angle This is the angle away from the cutting side of the tool. Front Angle This is thee angle on the cutting side of the tool. It does not matter if you reverse the values for Back and Front angle because SURFCAM can determine which is which. Clearance This is the value of the angle, from the cutting edge of the tool, that SURFCAM uses to prevent the side of the tool from touching the part in certain cuts. Orientation The tool Orientation box is informational on the Select Lathe Tool dialog box. It shows the default value that was entered when the selected tool was originally entered in the lathe tool library using the Lathe Tool Information dialog box (described in the following section). Default Operation The default operation that is performed by this tool. This default value is entered in the Lathe Tool Information dialog box. 5.1.2.2 Edit or Add a Lathe Tool New tools can be added to the lathe tool library. Features of existing tools can be edited. Click the Edit and Save button or the Add a Lathe Tool button on the Select Lathe Tool dialog box toolbar to display the Lathe Tool Information dialog box. Figure 8: Edit and Save Figure 9: Add a Lathe Tool

SURFCAM Reference Manual, Chapter 5 Lathe 303 Figure 10: Use this dialog box to edit a tool or to add a new lathe tool to the library. Reference Number The tool reference number. This number is used to look up the tool in the lathe tool library and must be unique. (Hint: Choose a reference number before clicking the button to open this dialog box. There are usually unused reference numbers following each group of tools. Use one of these numbers when adding new tools to the list.) The reference number must be between 1 and 255. Tool Description The description of the tool as it is to appear in the lathe tool list box on the Select Lathe Tool dialog box. This is limited to 40 characters. (The default descriptions provided include information such as the size and tool material type.) Tool Number, Length Offset, and Diameter Offset Enter appropriate values. Tool Material Choose from High Speed Steel, Carbide, TIC/TIN Coated Carbide, Cobalt HSS, TIC/TIN Coated HSS, Ceramic, Diamond, and Tapping. Default Coolant Choose the default coolant to be used with the tool. This can be Off, Flood, Mist, Flood Low Pressure, Flood High Pressure, Through Low Pressure, or Through High Pressure.

304 SURFCAM Reference Manual, Chapter 5 Lathe Program To Tool The tool is programmed to the Tip or the Center of the tool. Tool Tip and Center of Tool Radius Tool path using the Center option Tool path using the Tip option Figure 11: Tip or Center of Tool Drawing Files Specify the files used to draw the tool and the tool holder. When tool paths are being drawn, you can press the tab key to toggle through displaying just the tool, the tool and the tool holder, or neither the tool nor the holder. The file in the Tool list box contains the design for the tool. The files in the Holder and the three Other list boxes are combined together by SURFCAM to create the drawing of the tool holder.

SURFCAM Reference Manual, Chapter 5 Lathe 305 Click the... button to display the Select Tool Drawing File dialog box which is used to select an existing tool file. Figure 12: Select Tool Drawing File dialog box These tool files are design files in the same format as a DSN file except that they are given the.tle file extension for English inch tools or the.tlm file extension for metric tools. The default directory for storing TLE or TLM files is C:\SURFCAM\ Tool. Nose Radius, Radius, Inscribed Circle, Groove Width, Back Angle, Front Angle, Clearance Refer to Lathe Tool Parameters on page 301 for a description of these parameters. Turret Number The turret number for the tool. Chip Load The chip load on the tool in one revolution. Rough Depth The default rough cutting depth. Finish Depth The default finish cutting depth. Orientation The name of the tool orientation. The following drawings show the tool orientations for lathe tools and lathe groove tools and their names. Orientation determines the position of the programming point for Center and Tip programming modes.

306 SURFCAM Reference Manual, Chapter 5 Lathe Figure 13: Lathe tool orientation Lathe tool orientation numbers for other than groove tools are in the range of 0 to 7.

SURFCAM Reference Manual, Chapter 5 Lathe 307 Figure 14: Groove tool orientation Groove tool orientation numbers are also in the range of 0 to 7. However, in the tool library there is a flag. When tool path information is stored in the ICD file, a 20 is added to the groove tool numbers, making the actual groove tool number range 20-27. Default Operation The default operation that is performed by this tool. This default value is entered in the Lathe Tool Information dialog box. 5.1.2.3 Select a Lathe Drill Tool To select the tool to be used in a Lathe Drill operation, click the button to the right of the tool description on the Tool Information tab.

308 SURFCAM Reference Manual, Chapter 5 Lathe A Select Lathe Drill Tool dialog box will be displayed. Refer to the SURFCAM Getting Started Manual, Chapter 3: Common NC Parameters, Section 3.2.1.1: Select Tool on page 70 for a description of the four uses of the Select Tool dialog box. Figure 15: Select Lathe Drill Tool dialog box Toolbar Use the toolbar to select a tool, add a new tool, or edit the features of an existing tool. Go to first record. Choose drill reamer tool. Go to previous record. Go to next record. Go to last record. Choose drill center tool. Choose drill tool. Choose drill tap tool. Choose drill boring tool. Choose custom tool. Choose spot drill tool. Add a drill tool to the library. Edit / Save the current tool information. Delete the current tool record. Figure 16: Toolbar buttons on the Select Lathe Drill Tool dialog box Tables This box is available so you can select from different tool tables that you might have.

SURFCAM Reference Manual, Chapter 5 Lathe 309 Available Tools This list box will display the available tools of the currently selected class of lathe drill tools drill center, drill, drill tap, drill reamer, or drill boring. The tool reference number and description appear in the list. Selecting a tool in the list selects its parameters for the next NC lathe operation. You can change any of these tool parameters in the text fields of this dialog box before clicking OK. Tool parameter changes affect only the current operation and are not saved in the lathe tool library. Lathe Drill Tool Parameters The lathe drill tool parameters that can be changed are displayed next to the Available Tools list box. Drill Center Figure 17: Drill Parameters Drill

310 SURFCAM Reference Manual, Chapter 5 Lathe Drill Tap Drill Reamer Drill Boring Spot Drill Figure 17: Drill Parameters (Continued)

SURFCAM Reference Manual, Chapter 5 Lathe 311 5.1.2.4 Edit or Add a Lathe Drill Tool Refer to Section 5.1.2.2: Edit or Add a Lathe Tool on page 302 for details. New tools can be added to the lathe drill tool library; existing tools can be modified. Click the Edit and Save button or the Add a Drill Tool button to display the Drill Tool Information dialog box. Figure 18: Edit and Save Figure 19: Add a Drill Tool Figure 20: Lathe Drill Tool Information dialog box Spin The Spin check box next to each item under Drawing Files is used to specify whether or not the tool will spin while being displayed. 5.1.3 Turn Control Tab The cut control tabs for the Turn and Face operations Turn Control and Face Control are identical. The cut control tabs for the remaining lathe operations contain many of the same parameters that appear on the Turn Control tab. You will be referred to this section in the following sections that describe lathe operations.

312 SURFCAM Reference Manual, Chapter 5 Lathe Figure 21: Turn Control tab Operation This parameter available for the Turn, Face, Face Off, Groove, and Thread operations identifies the direction of the lathe operation you selected. Selecting an operation will automatically set the Cut, Retract, Lead In, and Lead Out angles to the standard angles for that operation. Click the arrow to open a drop-down list of operations specific to the lathe operation you chose on the Lathe menu. TURN OPERATIONS * FACE AND FACE OFF OPERATIONS * OD Turn OD Back Turn ID Back Bore ID Bore OD Face OD Back Face ID Back Face ID Face

SURFCAM Reference Manual, Chapter 5 Lathe 313 GROOVE OPERATIONS * THREAD OPERATIONS * OD Groove OD Right OD Back Groove OD Back Right ID Back Groove ID Back Right ID Groove ID Right OD Face Groove OD Left OD Back Face Groove OD Back Left ID Back Face Groove ID Back Left ID Face Groove ID Left * ID = Inside Diameter. OD = Outside Diameter. Cutter Compensation There are four types of cutter compensation available. Each has a corresponding method to include the machine control s code, for compensation. (G41/G42) The actual output will vary depending on the compensation method and whether the path is programmed to the tip or center. None This method outputs the coordinates of the chained geometry REGARDLESS of the Tip or Center option. The output code will not include G41/G42 codes. Figure 22: Cutter Compensation set to None, Programmed to Tip

314 SURFCAM Reference Manual, Chapter 5 Lathe Figure 23: Cutter Compensation set to None, Programmed to Center SURFCAM This method outputs the coordinates of the compensated insert BASED on the Tip or Center option. The output code will not include G41/G42 codes. The following two drawings are examples of the tool motion using the SURFCAM option. Figure 24: Cutter Compensation set to SURFCAM, Programmed to Tip

SURFCAM Reference Manual, Chapter 5 Lathe 315 Figure 25: Cutter Compensation set to SURFCAM, Programmed to Center Control This method differs from None in only one respect: the output will include G41/ G42. Both This method differs from SURFCAM in only one respect: the output will include G41/G42. Undercut The Undercut option provides control over the tool motion when an undercut (a groove or valley) exists along the chained profile. When set to No, SURFCAM ignores all undercuts in the chained path. When set to Yes, SURFCAM will cut only that part of an undercut that can be cut without gouging the surrounding material. Set to No Set to Yes Figure 26: Undercut

316 SURFCAM Reference Manual, Chapter 5 Lathe Curve Tolerance SURFCAM will break all contour moves along a spline into linear moves along chords connecting points on the spline. When driving the tool around a spline curve, SURFCAM will adjust the length of the chordal moves to make sure that the edge of the contour is never a greater distance from the chord than the value of the Curve Tolerance. Retract Clearance Before positioning to the start of the next pass, move to this distance above the highest point of the previous pass. Plunge Clearance The distance the tool will travel in a rapid move to the beginning of a tool path or away from the end of a tool path measured along a direction parallel to the retract direction. Side Clearance This is the cutter compensation value. Stock To Leave X and Z Enter the amount of stock to leave on the part for each axis. Rough and/or Finish Cut Use this parameter to set the cut to be a Rough Cut, Finish Cut, or Both. Front and back angle gouge checking is automatically applied to all rough and finish tool paths. SURFCAM uses the user-defined angles from the cutting edge of the tool to perform gouge checking. Set these angles in the tool library. To insure proper gouge checking, the tool library must be updated to your actual tools. The following drawings show the gouge checking for Rough and Finish cuts. Figure 27: Turn Gouge Checking

SURFCAM Reference Manual, Chapter 5 Lathe 317 Figure 28: Face Gouge Checking Rough Depth Of Cut This is the amount of material to remove on each roughing pass. This amount does not affect the Finish operation. This parameter is available only if you have selected Rough Cut or Both. Finish Depth Of Cut This is the amount of material to remove on each finish pass. This parameter is available only if you have selected Finish Cut or Both. The operation that you select in the Operation parameter sets the default values for the following parameters. You can override these values. Cut This angle determines the direction of tool motion. An angle of 180 causes the tool to cut from right to left. This parameter is available only if you have clicked Rough Cut or Both. It is not available for Finish Cut. Retract Enter the angle for the retract moves. Lead In / Lead Out Angle Set the angle for all Lead In and Lead Out moves. The Lead In move precedes the starting cut position. The Lead Out move follows the end of the cut. Length Set the length of the Lead In (Lead Out) move. Finish Passes The number of Finish Passes to perform. The Finish Depth Of Cut value is used on each of these passes. This parameter is available only if you have selected Finish Cut or Both. Spring Passes Indicate the number of extra times the final Finish Pass is cut. The final Finish Pass can be repeated to remove material that may be left due to part and/or tool deflection. This parameter is available only if you have selected Finish Cut or Both. Figure 29: Angular Definition This drawing assumes machining in View 1 Negative angles are supported

318 SURFCAM Reference Manual, Chapter 5 Lathe 5.1.4 Lathe Options Tab The Lathe Options tabs for all lathe operations contain the same set of parameters. Figure 30: Lathe Options tab Corner Angle A corner angle on a part is an angle between adjacent linear sections of a part contour or boundary. Corner angles can be located along the outside contour or along a pocket contour. SURFCAM creates toolpaths by creating offsets from the contour or sides of a part. The offsets around a corner angle will be two lines that may or may not intersect. If they intersect, as in the case of corner angles greater than 180, the tool path will merely change linear direction at the intersection. Offsets of corner angles between 150 and 180 will not intersect but SURFCAM automatically extends them so they do. The toolpath will then change direction at this intersection. The Corner Angle parameter tells SURFCAM how to fill the offset gap when a corner angle is less than 150. If a corner angle is less than 30, SURFCAM will close the gap between the two offsets by inserting an arc or several lines, depending on your selection in the box to the right of the Corner Angle box.

SURFCAM Reference Manual, Chapter 5 Lathe 319 When a corner angle is in the range of 30 to 150 and is less than the value you enter for Corner Angle, SURFCAM will close the offset gap with an arc or several lines, depending on your selection in the box to the right of the Corner Angle box. Figure 31: For an interior angle < 30ƒ an arc or line move will be inserted automatically Figure 32: For an interior angle > 150ƒ the consecutive line moves will automatically be intersectional Arc Figure 33: Example of two line moves that are intersectional An arc move will be inserted between line moves when the directional change is less than the Corner Angle value. The Corner Clearance value determines the location of the arc. Figure 34: Arc move inserted between line moves

320 SURFCAM Reference Manual, Chapter 5 Lathe Line A line move will be inserted between line moves when the directional change is less than the Corner Angle value. The Corner Clearance value determines the line location. Figure 35: Line move inserted between line moves Corner Clearance When an arc or line move is inserted (because the interior angle of a direction change is less than the Corner Angle value), this value determines the tool clearance from the direction change intersection. When this value is zero, the tool remains in contact with the part walls during the directional change. Groove Side Step (5-100%) The number entered here is the percentage that is used to calculate the value of the Groove Side Step parameter on the Groove Tool Information dialog box. This is a percentage of the flat part of the groove tool cutting surface. The flat part is equal to the groove tool width minus twice the tool nose radius of the tool. If the tool is not a groove tool, the interior circle of the tool multiplied by this percentage will be used. Figure 36: Flat part of groove tool cutting surface Lead In / Lead Out Speed Set the Lead In and Lead Out move speeds to Plunge, Feed or Rapid. Follow Sets the roughing pattern. When set to Yes, the roughing pattern follows the contour of the chained elements between roughing passes. When set to No, the roughing pattern steps in on the appropriate cutting angle for each pass. The following drawings show the same rough cut with this option set to Yes in the first picture and set to No in the second.

SURFCAM Reference Manual, Chapter 5 Lathe 321 Figure 37: Rough Cut with Follow set to Yes. The tool path follows the element contour between rough passes ToolLib Gauge Length This function is not implemented for Lathe operations. Figure 38: Rough Cut with Follow set to No. The tool path does not follow the element contour between rough passes 5.2 TURN The Turn operation is used most often to machine the part along the length of the material with cutting moves parallel to the Z axis. It can, in fact, be used to cut at any angle to the Z axis in the correct circumstances. Note: This section uses the X axis for diameters and the Z axis for lengths. The direction of the cutting moves are controlled by the Cut parameter on the Turn Control tab of the Lathe Turn dialog box. A Cut angle of 180 causes the cutting move to be from right to left or toward the chuck, while a Cut angle of zero causes moves in the opposite direction. A Cut angle of -90 causes moves toward the center line or Z axis, while 90 causes moves away from the Z axis. Other moves, such as Retract, Leadin and Leadout are measured in the same way. The Turn operation has four turning options. Two, called OD Turn and OD Back Turn, are outside diameter (OD) cutting operations. The other two, called ID Bore and ID Back Bore, are inside diameter (ID) cutting operations. The Operation parameter on the Turn Control tab identifies which of these turning operations will be used. The Operation parameter and the angle values for the Cut, Retract, Leadin and Leadout parameters are connected in that a change in the Operation parameter produces a corresponding change in the default setting for these other parameters, as shown in the following table: OPERATION CUT ANGLE RETRACT ANGLE LEADIN ANGLE LEADOUT ANGLE OD Turn 180 90 180 60 OD Back Turn 0 90 0 120 ID Back Bore 0-90 0-120 ID Bore 180-90 180-60

322 SURFCAM Reference Manual, Chapter 5 Lathe The Tool parameter, on the Tool Information tab, and the Operation parameter, on the Turn Control tab, are also connected in that the selection of a tool will cause the Operation parameter to be set to the operation for which that tool is most intended. To access the Turn operation click Turn on the NC Lathe menu. The Turn Chain menu will be displayed and you will be prompted to Select beginning element of part. Accurate chaining is important in defining the part contour that is to be turned. When selecting the beginning element of that contour, make sure you click on or near the beginning of the element. Remember that when you pick the beginning element you are selecting both a point and a direction for chaining the direction being from the beginning of the element toward the point you select. You will next be prompted to Select ending element of part. Pick the point at the other end of the contour that defines the area to be turned. You will then be prompted to Select beginning (ending) element of material boundary. Selecting the material boundary is optional. Either click Done or select the material boundary. SURFCAM will then display the Lathe Turn dialog box. Refer to 1. Section 5.1.2: Tool Information Tab on page 297, 2. Section 5.1.3: Turn Control Tab on page 311, and 3. Section 5.1.4: Lathe Options Tab on page 318. After you click OK on the Lathe Turn dialog box, SURFCAM will prompt you to Pick Lathe Retract Point and Pick Lathe Clearance Point. Refer to Retract-Clearance Points on page 296. After you select Retract and Clearance points SURFCAM will produce the toolpath and display it on the screen. It will then display the Keep Operation dialog box. Click Accept to keep the operation. To permanently save the toolpaths in the ICD file of your NC project, you must re-save the DSN file using the Save command on the Files menu. Figure 39: OD Turn with Cut angle = 180, Rough only Figure 40: OD Turn with Cut angle = 180, Finish only OD Turn: Cut angle = 180 with roughing and finishing machined separately

SURFCAM Reference Manual, Chapter 5 Lathe 323 ANGLE LENGTH Rough Depth Of Cut.25 Cut 180.00 Retract 90.00 Lead In 180.00.1 Lead Out 60.00.2 Figure 41: Rough OD Turning Operation ANGLE LENGTH Rough Depth Of Cut.25 Cut 180.00 Retract -90.00 Lead In 180.00.1 Lead Out -60.00.2 Figure 42: Rough ID Boring Operation ANGLE LENGTH Finish Depth Of Cut.01 Retract 90.00 Lead In 180.00.1 Lead Out 60.00.2 Finish Passes 1 Spring Passes 0 Figure 43: Finish OD Turning Operation

324 SURFCAM Reference Manual, Chapter 5 Lathe ANGLE LENGTH Finish Depth Of Cut.01 Retract -90.00 Lead In 180.00.1 Lead Out -60.00.2 Finish Passes 1 Spring Passes 0 Figure 44: Finish ID Boring Operation ANGLE LENGTH Rough Depth Of Cut.25 Finish Depth Of Cut.01 Cut 180.00 Retract 90.00 Lead In 180.00.1 Lead Out 60.00.2 Finish Passes 1 Spring Passes 0 Figure 45: OD Turning Operation with Rough and Finish ANGLE LENGTH Rough Depth Of Cut.25 Finish Depth Of Cut.01 Cut 180.00 Retract -90.00 Lead In 180.00.1 Lead Out -60.00.2 Finish Passes 1 Spring Passes 0 Figure 46: ID Boring Operation with Rough and Finish

SURFCAM Reference Manual, Chapter 5 Lathe 325 5.3 FACE The Face operation is used most often to machine the part along the diameter of the material with cutting moves perpendicular to the Z axis. It can, in fact, be used to cut at any angle to the Z axis in certain circumstances. Note: This section uses the X axis for diameters and the Z axis for lengths. The direction of the cutting moves is controlled by the Cut Angle parameter on the Face Control tab of the Lathe Face dialog box. A Cut Angle of -90 causes moves toward the center line, while 90 causes moves away from the center line. A Cut Angle of 180 causes the cutting move to be from right to left or toward the chuck, while a Cut Angle of zero causes moves in the opposite direction. The Retract, Leadin and Leadout moves are measured in the same way. The Face operation has four turning options. Two OD Face and OD Back Face are outside diameter (OD) cutting operations. The other two ID Face and ID Back Face are inside diameter cutting operations. The Operation parameter on the Face Control tab identifies which of these turning operations will be used. The Operation parameter and the angle parameters for the Cut, Retract, Leadin and Leadout moves are connected in that a change in the Operation parameter produces a change in the default setting for the angles as shown in the following table: OPERATION CUT ANGLE RETRACT ANGLE LEADIN ANGLE LEADOUT ANGLE OD Face -90 0-90 30 OD Back Face -90 90-90 120 ID Back Face 90-90 90-120 ID Face 90 0 90-30 The Tool Library # parameter and the Operation parameter are also connected in that the selection of a tool will cause the Operation parameter to be set to the operation for which that tool is most intended. To access the Face operation, click Face on the NC > Lathe menu. The Face Chaining menu will be displayed and you will be prompted to Select beginning element of part. Accurate chaining is important in defining the part contour that is to be turned. When selecting the beginning element of that contour, make sure you click on or near the beginning of the element. Remember that when you pick the beginning element, you are selecting both a point and a direction for chaining the direction being from the beginning of the element toward the point you select. You will next be prompted to Select ending element of part. Pick the point at the other end of the contour that defines the area to be turned.

326 SURFCAM Reference Manual, Chapter 5 Lathe You will then be prompted to Select beginning (ending) element of material boundary. Selecting the material boundary is optional. Either select the material boundary or click Done. SURFCAM will then display the Lathe Face dialog box. Refer to 1. Section 5.1.2: Tool Information Tab on page 297, 2. Section 5.1.3: Turn Control Tab on page 311, and 3. Section 5.1.4: Lathe Options Tab on page 318. After you click OK on the Lathe Face dialog box, SURFCAM will prompt you to Pick Lathe Retract Point and Pick Lathe Clearance Point. Refer to Retract-Clearance Points on page 296. After you select Retract and Clearance points SURFCAM will produce the toolpath and display it on the screen. It will then display the Keep Operation dialog box. Click Accept to keep the operation. To permanently save the toolpaths in the ICD file of your NC project, you must re-save the DSN file using the Save command on the Files menu. Figure 47: OD Face turn with Cut angle = -90, Rough only Figure 48: OD Face with Cut angle = -90, Finish only The facing operation with roughing and finishing machined separately. ANGLE LENGTH Rough Depth Of Cut.150 Cut -90.00 Retract 0.00 Lead In -90.00 0 Lead Out 30.00 0 Figure 49: Rough OD Face: Cut angle = -90

SURFCAM Reference Manual, Chapter 5 Lathe 327 ANGLE LENGTH Rough Depth Of Cut.250 Cut 90.00 Retract 0.00 Lead In 90.00.1 Lead Out -30.00.2 Figure 50: Rough ID Face: Cut angle = 90 ANGLE LENGTH Finish Depth Of Cut.010 Retract 0.00 Lead In -90.00.1 Lead Out 30.00.2 Finish Passes 1 Spring Passes 0 Figure 51: Finish OD Face: Cut angle = -90 ANGLE LENGTH Finish Depth Of Cut.010 Retract 0.00 Lead In 90.00.1 Lead Out -30.00.2 Finish Passes 1 Spring Passes 0 Figure 52: Finish ID Face: Cut angle = 90

328 SURFCAM Reference Manual, Chapter 5 Lathe ANGLE LENGTH Rough Depth Of Cut.250 Finish Depth Of Cut.010 Cut -90.00 Retract 0.00 Lead In -90.00.1 Lead Out 30.00.2 Finish Passes 1 Spring Passes 0 Figure 53: OD Face with Rough and Finish Cut angle = -90 ANGLE LENGTH Rough Depth Of Cut.250 Finish Depth Of Cut.010 Cut 90.00 Retract 0.00 Lead In 90.00.1 Lead Out -30.00.2 Finish Passes 1 Spring Passes 0 Figure 54: ID Face with Rough and Finish Cut angle = 90 5.4 FACE OFF The Face Off operation is used to remove material from the face of the part in preparation for performing other turning operations. You can remove a specified amount of material to the right of a point you select on the part. Most of the time this point will be the right most point on the part. In addition to a point on the face of the part and the amount of material to remove, you must identify a point on the outside diameter of the material and one on the inside diameter. The inside diameter of the material will usually be the Z axis so that all the material on the face of the part will be removed. However, if you work with stock that has a hole in its center, you might want to identify a point on the inside of the hole as the inside diameter in order to avoid unnecessary tool moves. The outside and inside diameters referred to above, are called the major and minor diameters, and when you perform the Face Off operation, SURFCAM will prompt you to select them. The amount of material to remove is identified in the Stock To Remove parameter on the Face Off Control tab. To access the Face Off operation click Face Off on the NC > Lathe menu. The Select Point Menu will be displayed and you will be prompted to Select a point on the face. Select one of the right

SURFCAM Reference Manual, Chapter 5 Lathe 329 most points on the part. You will then be prompted to Select a point denoting major diameter or Done for prev point position. Select a point on the outermost diameter of your material. If that point is the same as the one you selected as a point on the face, you can click Done to use the previously selected point. You will then be prompted to Select a point denoting minor diameter or Done for 0. Select a point that identifies the innermost diameter to which you want to cut. If the point is on the Z axis, you can click Done. SURFCAM will then display the Lathe Face Off dialog box. Refer to Section 5.1.2: Tool Information Tab on page 297 and Section 5.1.4: Lathe Options Tab on page 318. Following is the Face Off Control tab. Figure 55: The Face Off Control tab For a description of the parameters not in the following list, refer to Section 5.1.3: Turn Control Tab on page 311. Stock to Remove Enter the amount of stock to remove from the part. Minor Diameter The distance from the Z axis to the inner most point on the material. Unless the inner most part of the stock contains a hole the Minor Diameter will have a value of zero.

330 SURFCAM Reference Manual, Chapter 5 Lathe Major Diameter The distance from the Z axis to the outermost part of the stack. There are three key parameters for the Face Off operation: the Tool parameter on the Tool Information tab and the Operation and Stock To Remove parameters on the Face Off Control tab. First, you must select a tool from the tool library. When you do, the Operation parameter is set to the appropriate operation. Indicate the amount of material to remove from the right side of the part by entering the value in the Stock to Remove field. After you click OK on the Lathe Face Off dialog box, SURFCAM will prompt you to Pick Lathe Retract Point and Pick Lathe Clearance Point. Refer to Retract-Clearance Points on page 296. After you select Retract and Clearance points SURFCAM will produce the toolpath and display it on the screen. It will then display the Keep Operation dialog box. Click Accept to keep the operation. To permanently save the toolpaths in the ICD file of your NC project, you must re-save the DSN file using the Save command on the Files menu. 5.5 GROOVE The Groove operation is used to cut grooves in a part. There are several categories of groove cutting available: OD Groove, OD Back Groove, ID Back Groove, ID Groove, OD Face Groove, OD Back Face Groove, ID Back Face Groove, and ID Face Groove. Select the category you want to use with the Operation parameter on the Tool Information dialog box. Note: This section uses the X axis for diameters and the Z axis for lengths. To access the Groove operation click Groove on the NC > Lathe menu. The Groove chaining menu will be displayed and you will be prompted to Select beginning element of part. Accurate chaining is critical to defining the groove. When selecting the beginning element of the groove, make sure you click on a point that is near the beginning of the element. Remember that when you pick the beginning element you are selecting both a point and a direction for chaining the direction being from the beginning of the element toward the point you select. You will next be prompted to Select ending element of part. Pick the point at the other end of the contour that defines the groove. You will then be prompted to Select beginning element of material boundary. Selecting the material boundary is optional. Either select the material boundary or click Done. SURFCAM will then display the Lathe Groove dialog box. Refer to Section 5.1.2: Tool Information Tab on page 297 and Section 5.1.4: Lathe Options Tab on page 318.

SURFCAM Reference Manual, Chapter 5 Lathe 331 Following is the Groove Control tab. Figure 56: Groove Control tab Refer to Section 5.1.3: Turn Control Tab on page 311. Rough Cycle Type Cycle type describes the way in which succeeding tool moves are performed when cutting a groove. Two Cycle Types use the center of the groove. The center is defined to be either the lowest point in the groove or, if the lowest point lies on a horizontal line, the center of that line. Center Sequential The first move is down the center of the groove. The next moves are toward one edge of the groove (to the left for OD groove). When the first half of the groove is cut, the tool returns to the center and moves toward the other edge (to the right for OD groove). Center Alternate The first move is down the center of the groove. The next move is to one side of the center (to the left side for OD groove), followed by a move on the other side. The cutting moves alternate from one side of the center to the other until the groove is complete.

332 SURFCAM Reference Manual, Chapter 5 Lathe Sequential The first move is down one edge of the groove (the right edge for OD groove). The next moves are in the direction of the other edge (to the left for OD groove). Groove Side Step The distance that the tool steps over to make the next cutting pass. It is a calculated value. Refer to Groove Side Step (5-100%) on page 320. Finish Cycle Finish cycle describes the sequence of tool moves performed when doing finish cutting. Groove To Center The first finish move is down one edge of the groove (the right edge for OD groove) to the bottom and then over to the center. The next move is down the other edge, and then over to the center of the groove. Groove To Face The first move is down one edge of the groove to the bottom (the left edge for OD groove). The next move is down the other edge to the bottom and then over to the other edge. After you click OK on the Lathe Groove dialog box, SURFCAM will prompt you to Pick Lathe Retract Point and Pick Lathe Clearance Point. Refer to Retract-Clearance Points on page 296. After you select Retract and Clearance points SURFCAM will produce the toolpath and display it on the screen. It will then display the Keep Operation dialog box. Click Accept to keep the operation. To permanently save the toolpaths in the ICD file of your NC project, you must re-save the DSN file using the Save command on the Files menu. 5.6 THREAD The Thread operation is used to create inside or outside canned cycle threads. This operation performs the rough and finish cuts for the thread. To access the Thread operation, click Thread on the NC > Lathe menu. You will be prompted to Select a line for lathe thread. Click on a line on your drawing along which you want a thread to be cut. After you select the line to thread, the Lathe Thread dialog box will be displayed. Refer to Section 5.1.2: Tool Information Tab on page 297 and Section 5.1.4: Lathe Options Tab on page 318.

SURFCAM Reference Manual, Chapter 5 Lathe 333 Following is the Thread Control tab. Figure 57: Lathe Thread Control tab Operation The available thread operations are OD Right, OD Back Right, ID Back Right, ID Right, OD Left, OD Back Left, ID Back Left, and ID Left. Thread Pitch Enter the distance from one thread to the next. This can be entered as Thread per inch (TPI) or Inches per thread (IPT) if you are using metric, Millimeters per thread (MPT) or Threads per Millimeter (TPM). Inches per thread is calculated as 1 / number of threads per inch. Depth of Thread The distance from the major radius of the thread to the minor radius. Do not use the thread diameter. The default value is calculated from the thread pitch. If you change the thread pitch, the depth will be re-calculated and changed also. First Cut Depth This is the initial material removal amount per side. Minimum Cut Depth Indicates the minimum amount of material to remove for any pass.

334 SURFCAM Reference Manual, Chapter 5 Lathe Infeed Angle Enter the angle for the infeed move. The angle is measured from vertical. Retract Angle Enter the angle for the retract move. The angle is measured from vertical. Retract Clearance Enter the distance above the top of the thread to retract to, before positioning to the next pass. This move is made at the retract angle. Figure 58: Included Angle and Thread Angle Starts A multiple start thread is a thread in which the lead is an integral multiple, other than one, of the pitch. For this option, enter the number of starts for the thread. Spring Passes The number of times the final finish pass is re-cut. The final finish pass can be repeated to remove material that may be left due to part and/or tool deflection. Lead In Length Enter the distance for the approach to the first thread. This value can be entered as threads or inches (millimeters). Lead Out Length Enter the distance to overrun the last thread to insure a complete thread. This value can be entered as threads or inches (millimeters). After you click OK on the Lathe Thread dialog box, SURFCAM will prompt you to Pick Lathe Retract Point and Pick Lathe Clearance Point. Refer to Retract-Clearance Points on page 296. After you select Retract and Clearance points SURFCAM will produce the toolpath and display it on the screen. It will then display the Keep Operation dialog box. Click Accept to keep the operation. To permanently save the toolpaths in the ICD file of your NC project, you must re-save the DSN file using the Save command on the Files menu. 5.7 DRILL The Drill command on the NC > Lathe menu is used to drill the face of the part. Only the part centerline can be drilled. When you click Drill on the NC > Lathe menu, the Select Point menu will be displayed and you will be prompted to Select starting location for canned cycle. After you select the location to drill, the Lathe Drill dialog box will be displayed.

SURFCAM Reference Manual, Chapter 5 Lathe 335 Refer to Section 5.1.2: Tool Information Tab on page 297 for a description of the Drill Tool Information tab parameters except for Tool Diameter and Number of Flutes. These are values that are loaded from the tool library when a drill tool is selected. For a description of the Lathe Options, refer to Section 5.1.4: Lathe Options Tab on page 318. Figure 59: Lathe Drill Control tab Cycle Type Refer to the SURFCAM Getting Started Manual, Chapter 4: Common NC Operations, Cycle Type on page 102. Hole Depth This is the depth of the hole from the geometry described. Depth To This controls which part of the drill is taken to the depth defined by Hole Depth. Tip Tip will take the tip of the drill to the defined depth. Center Center will take the full diameter of the drill to the defined depth.

336 SURFCAM Reference Manual, Chapter 5 Lathe Drill Included Angle Drill Included Angle is active when the Depth To parameter is set to Center. This is the tool Tip Angle. The default value for a standard twist drill is 118. The default value for each drill in the tool library file can be changed in the Drill Tool Information dialog box which is accessed by clicking the Edit and Save button on the Select Lathe Drill Tool dialog box. Refer to the SURFCAM Getting Started Manual, Chapter 3: Common NC Parameters, Section 3.2.1.1: Select Tool on page 70. Clearance Define an extra distance for the overall depth of the hole. This can make up for a drill that has rounded edges and can break the edge to reduce deburring. Initial Rapid This is the absolute Z plane for the beginning of the drill cycle. Refer to Figure 60: Initial Rapid, Plunge Clearance, and Clearance Position. Plunge Clearance This is the relative distance above the top of the hole at which the tool should start moving at feed rate. The tool will move at rapid speed from the Initial Rapid plane to the Plunge Clearance point. Figure 60: Initial Rapid, Plunge Clearance, and Clearance Position Retract To This is the level to which the drill will retract at the end of the drill cycle. Rapid Plane This is a G98 type move using the value entered for Initial Rapid. Plunge Clearance This is a G99 type move using the value entered for Plunge Clearance.

SURFCAM Reference Manual, Chapter 5 Lathe 337 Dwell time Enter the length of time to dwell for the appropriate cycle. This time is entered in milliseconds (1000 = 1 second). Peck Increment Enter the peck size for the peck cycle. Bore Side Clearance This is the side clearance for the bore cycles. After you click OK on the Lathe Drill dialog box, SURFCAM will prompt you to Pick Lathe Retract Point. Refer to Retract-Clearance Points on page 296. After you select the Retract Point SURFCAM will produce the toolpath and display it on the screen. It will then display the Keep Operation dialog box. Click Accept to keep the operation. To permanently save the toolpaths in the ICD file of your NC project, you must re-save the DSN file using the Save command on the Files menu. 5.8 PARTOFF The Partoff operation is used to cut a turned part off of the bar stock from which it was machined. Click Partoff on the NC > Lathe menu. The Select Point Menu will be displayed and you will be prompted to Select a point on the back face. Select one of the left most points on the part. You will then be prompted to Select a point denoting major diameter or Done for prev point position. Select a point on the outermost diameter of your part. If that point is the same as the one you selected as a point on the back face, you can click Done to use the previously selected point. You will then be prompted to Select a point denoting minor diameter or Done for 0. Select a point that identifies the innermost diameter to which you want to cut. If the point is on the Z axis, you can click Done. SURFCAM will then display the Lathe Partoff dialog box. Refer to Section 5.1.2: Tool Information Tab on page 297 and Section 5.1.4: Lathe Options Tab on page 318 for descriptions of parameters on the Tool Information and Lathe Options tabs. Refer to Section 5.1.3: Turn Control Tab on page 311 for descriptions of parameters on the Partoff Control tab that are not described here.