Transcript
M570
1
Operating mode “JOG“
Brief description
Objective of the module: In this module you learn the different options of the operating area "Machine" in the operating mode "JOG". Description of the module: In this module the softkeys of the Sinumerik Operate, available in the manual mode (setup- and basic functions), will be described. Content: Operating mode "JOG" Tool, spindle and machine commands (T,S,M) Set Work offset (“Set WO”) Measure workpiece Measuring a tool Position Face milling Settings
828D/840Dsl SINUMERIK Operate 828D/840Dsl SINUMERIK Operate
Page 1
This document was produced for training purposes. Siemens assumes no responsibility for its contents.
M570
M570
M570
Page 2
828D/840Dsl SINUMERIK Operate
M570 Operating mode JOG: Description In this module the softkeys of the Sinumerik Operate, available in the manual mode (setup and basic functions), will be described.
Operating mode JOG: START
Operating mode "JOG"
Tool-, spindleand machine commands (T,S,M)
Set Work offset (“Set WO”)
Measure workpiece
Measuring a tool
Position
Face milling
Setting
Operating mode JOG: END
Notes
828D/840Dsl SINUMERIK Operate
Page 3
M570
Section 2 Notes
Operating mode “JOG“ Operation mode “JOG” is used, for setting up the machine for program runoff or if you simply want to traverse the axes on the machine: Reference point approach, i.e. calibration of the position measuring system Preparing a machine for executing a program in automatic mode, i.e. measuring tools, measuring the workpiece and, if necessary, defining the work offsets used in the program Traversing axes, e.g. during a program interruption Positioning axes 2.1
Selecting the operating mode “JOG“
The operating mode "JOG" can be selected as follows: Press the “JOG“ button on the machine control panel (MCP). The operating mode “JOG” opens directly. - OR Press the button “MENU SELECT“ on the machine control panel. Press the VSK 1 “JOG“ in the yellow vertical softtkey bar on the right hand side of the screen to switch directly to the operating mode “JOG“. Then Switch to the operating area “Machine” by pressing the “MACHINE” key on the operator panel or on the keyboard or press the “MENU SELECT“key on the operator panel and the yellow HSK 1 “Machine“. The following screen opens:
M570
Page 4
828D/840Dsl SINUMERIK Operate
Operating mode “JOG“
Section 2
The following functions are offered in the horizontal and vertical softkey bar of the operating area "Machine" ( see section 2.2 and 2.3). 2.2
Notes
Vertical softkey bars 1 and 2
Display area
Description The most important G-functions are displayed in a sub-window by pressing the VSK 1.1 "G functions". Available auxiliary functions are displayed in a subwindow by pressing the VSK 1.2 "Auxiliary functions" at the time of the output. By pressing the VSK 1.7 "Act. values. Machine", the coordinate system will be toggled between the machine coordinate system (MCS) and the workpiece coordinate system (WCS). Note: Refer to the machine manufacturer‘s documentation. By pressing the VSK 1.8 "Forward" on the operator panel (OP) the selection of additional softkeys on the vertical softkey bar is possible By pressing the VSK 2.2 "All G functions" all Gfunctions will be shown. By pressing the VSK 2.6 "Zoom act. val." all actual axes positions in the selected coordinate system as well as the currently active feed rate and feed override of each individual axis are displayed full screen. In addition all active zero point offsets, transformations and the T,F,S data is being displayed in the foot line. Note: If the machine is in the sub-mode “REPOS”, then the in manual mode traversed path difference is also being displayed. By pressing the VSK 2.8 "Back" on the operator panel (OP) the vertical softkey bar switches back to the menu of the VSK 1.
828D/840Dsl SINUMERIK Operate
Page 5
M570
Section 2 Notes
Operating mode “JOG“ 2.3
Horizontal softkey bar 1 and 2
Display area
Description By pressing the HSK 1 "T,S,M" the input screen "T,S,M" will be activated. By pressing the HSK 2 "Set WO" the input screen for setting the work offset will be activated. By pressing the HSK 3 "Meas. workp.“ the input mask for measuring a workpiece will be activated. By pressing the HSK 4 "Meas. tool" the function "Measure tool" will be activated and the extended options "Length/Radius manual", "Length/Radius auto", "Calibrate Probe", and “Calibrate fixed pt.” will be available in the vertical softkey bar. By pressing the HSK 5 "Position" the input screen "Target position" will be activated. By pressing the HSK 7 "Face mill." the input screen "Face milling" will be activated. By pressing the "Extend"-button on the operator panel (OP) more softkeys on the HSK are available.
This symbol on the right of the dialogue line indicates that more options on the HSK are available. This symbol indicates that you are in the expanded softkey bar. By pressing the HSK 2.6 "Handwheel" the input mask for traversing the axis in machine coordinate system (MCS) or workpiece coordinate system (WCS) will be available. By pressing the HSK 2.7 "Synch. Action." the screen which shows the current synchronized actions is displayed. By pressing the HSK 2.8 "Settings" a window opens up where you can adjust the settings for manual operation on the Sinumerik Operate.
M570
Page 6
828D/840Dsl SINUMERIK Operate
Tool, spindle and machine commands (T,S,M) 3.1
Selecting the function "T,S,M" (Tool, spindle and machine commands)
Section 3 Notes
By pressing the HSK 1 "T,S,M" in operation area “Machine” under operation mode “JOG” the following input mask will be displayed on the screen .
3.2
Vertical softkey bar (VSK)
Display area
Description By pressing the VSK 2 "Select tool" the tool list opens on the screen. See module M573 - "Operating area Parameter". By pressing the VSK 3 "Select work offs" a list with the zero point offsets will be displayed. Refer to Work offset section 4 in this module By pressing the VSK 8 "Back" switch back to the main screen of the Sinumerik Operate.
828D/840Dsl SINUMERIK Operate
Page 7
M570
Section 3 Notes
Tool, spindle and machine commands (T,S,M) 3.3
Parameters of "T,S,M" (Tool, spindle and machine commands)
Input mask for tool-, spindle- and machine commands: Values can be entered directly in the orange marked input fields or by selecting predefined parameters with the “SELECT”-key. Alternatively the “INSERT”-button in the marked cursor field opens a select menu of all possible parameters, in which you can navigate with the “Tab”key as well as the blue “cursor-up”- and “cursor-down”-down buttons. The button “INPUT” takes over the selected values. In order to be independently of country specific measuring units [metric/ imperial] not all units are displayed in the input masks. See module M568 - "Basic operations". In this documentation the measuring units are always metric.
Parameter
Unit
Meaning
T
Tool name: e.g.: T12 or Cutter_7 (alphanumerical).
D
Cutting edge number of the tool.
Spindle:
[rpm]
Spindle speed (revolutions per minute, numerical). Spindle machine functions: (Make a selection using the "SELECT"-key on the keyboard).
Spindle M function: Empty field
No selection is made. Right(M 3) Clockwise rotation of the spindle. Left (M 4) Counter clockwise rotation of the spindle. Off (M 5) Spindle is stopped. Positioning (SPOS)
Spindle positioning: Spindle is positioned to the desired position. Manufacturer defined M-functions. By inserting the number of the function, a corresponding M-function is selected.
Other M function:
Refer to the machine manufacturer‘s table for the correlation between the meaning and the number of the function.
M570
Page 8
828D/840Dsl SINUMERIK Operate
Tool, spindle and machine commands (T,S,M) Parameter
Unit
Meaning (continuation)
Section 3 Notes
Alternative parameter options: The actual value of the work offset refers to the machine zero point, after approaching the reference point.
Work offset: None Basic reference
In contrast a machining program refers to the workpiece zero point. This offset is to be entered as zero point offset.
G54 G55
You can select work offsets from the tool list of settable work offsets via the "Work offset" softkey.
G56 G57
See module M573 - "Operating area Parameter". Alternative parameter options:
Unit of measure.: none mm
[mm]
inch
[inch]
Note: The setting made here has effect on the programming.
Machining plane: G17
(XY)
G18
(ZX)
G19
(YZ)
Gear stage:
Specification of the gear stage (none, auto, I - V).
Stop-Position:
[Degree]
Input of the spindle position in degrees. Note: This parameter shows up by selecting the spindle M-function .
Note: With “CYCLE START“ the inserted values will be executed. The entries in the option fields will be deleted, ready for new inputs. 828D/840Dsl SINUMERIK Operate
Page 9
M570
Section 3 Notes
Tool, spindle and machine commands (T,S,M) 3.4
Tool definition and call with the input mask "T, S, M"
By pressing the HSK 1 "T, S, M" on the screen See above in the working window open the "T, S, M" input box. The VSK 1 "Select tool" Softkey appears. Pressing this soft key will open the tool list.
M570
Page 10
828D/840Dsl SINUMERIK Operate
Tool, spindle and machine commands (T,S,M) Press VSK 1 "New tool" Softkey to open the “Favorites” tool selection.
Section 3 Notes
Opened by default, VSK 1 "Favorites" Softkey, you will find the most common tools. By pressing on the soft keys such as "Drill", only drilling tools are offered. In our example, the first tool "Type 120 - End mill" is used.
With the VSK 8 "OK" Softkey, the selected tool is created in
The name of the tool can be modified if required. For example, the tool name is edited from MILLING CUTTER with the Insert and Delete keys and changed to CUTTER_D10.
828D/840Dsl SINUMERIK Operate
Page 11
M570
Section 3 Notes
Tool, spindle and machine commands (T,S,M) Data should now be entered if known, the tool length, the correct tool radius or diameter, and number of edges, spindle direction and possibly external coolant supply can be activated.
Press VSK 1 "In Manual", the tool name is now moved into the input window of T, S, M.
The tool could also have speed and direction data entered, if it is still stored in the magazine. In this example CYCLE START is pressed to initiate the tool change.
CYCLE START triggers the tool change functions without additional commands such as M06.
M570
Page 12
828D/840Dsl SINUMERIK Operate
Tool, spindle and machine commands (T,S,M)
Section 3 Notes
The tool should now appear in the window technology (outlined in red), the tool from the tool list with details of length, radius and edge number.
To return the tool in the spindle to the magazine must only be undertaken using "T, S, M" In the input field T enter "0".
CYCLE START triggers the tool change functions without additional commands such as M06.
828D/840Dsl SINUMERIK Operate
Page 13
M570
Section 4 Notes
Work offset 4.1
Selecting the function "Work offset" By pressing the HSK 2 "Set WO" in operation area “Machine” under operation mode “JOG” the input field for the programming of a work offset will be opened, like displayed below.
Input value:
By selecting an axis you can insert a value for the zero point offset in the orange marked field (see the picture above). The navigation through the axis-fields can be accomplished by pressing the blue “cursor-up“ and “cursor down“ keys on the keyboard. The slider on the right side of the sub window indicates that there are more axis values available, that can be reached by using the “cursor-down“ key.
Important:
The horizontal softkey 2 "Set WO" is only selectable if the workpiece coordinate system is selected and a zero point offset (in this example G54) is active. The entered values for a zero point offset of the axis will be accepted and displayed in the workpiece coordinate system (WCS). The difference between the original position to the new entered value will be written to the active zero point offset.
M570
Page 14
828D/840Dsl SINUMERIK Operate
Section 4
Set work offset (“Set WO”) 4.2
Notes
Vertical softkey bar
Display area
Description By pressing the VSK 1 "X=0" the position of the Xaxis will be reset to zero. By pressing the VSK 2 "Y=0" the position of the Yaxis will be reset to zero. By pressing the VSK 3 "Z=0" the position of the Zaxes will be reset to zero. By pressing the VSK 4 „X=Y=Z=0“ the position of the X/Y/Z-axis will be reset to zero. By pressing the VSK 5 "Delete active WO" the zero point offset of all axes is set back to zero. By pressing the VSK 8 "Back" you switch back to the main screen of the Sinumerik Operate.
Note: After setting a position or deleting a zero point offset you switch back automatically to the main screen of the Sinumerik Operate.
828D/840Dsl SINUMERIK Operate
Page 15
M570
Section 5 Notes
Measure workpiece 5.1
Selecting the function “Measure workpiece“ In the operating area “Machine“ under the operating mode “JOG“ press the HSK 3 "Meas. workp." to open the “Measure workpiece“ window shown below.
The reference point for programming a workpiece is always the workpiece zero. You can determine the workpiece zero on the following workpiece elements: Edges (Set edge, Align edge) Corner (Rectangular corner) Hole (1 Hole, 2 Holes, 3 Holes, 4 Holes)) Spigot (Circular spigot, rectangular spigot) The workpiece zero can be measured either manually or automatically. Measuring manually: For manual measuring their are parameters that depend upon tool type, and therefore are only available for the particular case. The tool must be manually approached to the workpiece. You can use edge probes, sensing probes, or dial gauges with known radii and lengths. You can also use any other tool of which you know the radius and length. The tools used for measuring must not be electronic probes. Measuring automatically: For automatic measurements always use electronic 3-D or mono workpiece probes. You must calibrate the electronic workpiece probes beforehand. First position the workpiece probe manually. As soon as you start the process with the "CYCLE START" key, the workpiece probe automatically approaches the workpiece at measuring feedrate and then returns to the starting position at rapid traverse. The machine manufacturer must first set the appropriate machine parameters (e.g. the measuring feedrate). Note: During all measurements the override of the feedrate should be set to 100%.
M570
Page 16
828D/840Dsl SINUMERIK Operate
Section 5
Measuring workpiece 5.2
Notes
Vertical softkey bar
Display area
Description By pressing the VSK 1 “Calibrate probe“ the input mask for “Calibrate probe“ opens. By pressing the VSK 2 “Set edge“ the “Set edge“ window opens. By pressing the VSK 3 “Align edge” the “Align edge” window opens. By pressing the VSK 4 “Rectangular corner” the “Rectangular corner” window opens. By pressing the VSK 5 “1 Hole” the “1 Hole” window opens. By pressing the VSK 6 “1 Circular spigot” the “1 Circular spigot” window opens. By pressing the VSK 8 "Back" you switch back to the main screen of the Sinumerik Operate.
5.3 Selecting the function “Calibrate probe” By pressing the HSK 3 “Meas. workp.” and the VSK 5 “Calibrate probe” (in operating area “Machine” and operating mode “JOG”) the following input screen will be displayed.
828D/840Dsl SINUMERIK Operate
Page 17
M570
Section 5 Notes
Measuring workpiece 5.4 Example of two measurement functions "Set edge" and "tap into rectangular"
As already described in Section 3, a mechanical probe to be created in the tool list and using "T, S, M" loaded into the spindle.
With the VSK 1 "In Manual", the tool is transfered into the input window of T, S, M.
Additional functions of the input mask of "T, S, M" are briefly explained. The "Spindle M function", a mechanical probe is oriented for easy reading. The "Stop position" can be any angle. In addition, the offset can be activated, in which the measured values are to be entered.
M570
Page 18
828D/840Dsl SINUMERIK Operate
Section 5
Measuring workpiece The technology window will display the measuring tool from the tool list, with details of length and edge number.
Notes
Note: The part to be measured is "Set edge" on the workpiece surface with the measurement function with 1mm oversize and is in the middle of the workpiece, measured with the measuring function "Rectangular spigot" . (This will be shown as an example in Section 5.4 and 5.5). 5.4
Measure workpiece zero “Set edge”
The workpiece lies parallel to the coordinate system on the work table. One reference point will be measured in one of the axes (“X”, “Y”, “Z”). The following requirements must be fulfilled: Any tool can be loaded in the spindle for scratching when measuring the workpiece zero manually. An electronic workpiece probe is loaded in the spindle and activated when measuring the workpiece zero automatically. By pressing the HSK 3 “Meas. workp.” and the VSK 2 “Set edge“, in the operating area “Machine“ and operating mode “JOG“, the following screen will be displayed.
828D/840Dsl SINUMERIK Operate
Page 19
M570
Section 5 Notes
Measuring workpiece 5.4.1 Vertical softkey bar (VSK) Display area
Description By pressing the VSK 2 “Select work offset“ a list of the work offsets opens. See module B573 - “Operating area Parameter“. By pressing the VSK 3 “X“ the measured values for the X-axis will be determined. By pressing the VSK 4 “Y“ the measured values for the Y-axis will be determined. By pressing the VSK 5 “Z“ the measured values for the Z-axis will be determined. By pressing the VSK 7 “Set WO“ the values will be accepted for the work offset. By pressing the VSK 8 “Back“ you switch back to the “Measure workpiece“ main screen .
5.4.2 Parameters of "Set edge" Parameter
Description
Work offset:
Alternative parameters
Measure only
The measured values are computed and displayed without changing the coordinate system.
Work offset
Measurement direction: X
Y
Z
Reference point
M570
The selection of the axes directions “X”/”Y”/”Z” is made by the vertical softkey bar. With the measurement direction (+ or -) it is determined whether the workpiece will be approached from a positive or negative “X”- or “Y”direction. By selection of the axis direction “Z it is only possible to approach the work piece from a negative Z-direction.
X0, Y0, Z0
Page 20
828D/840Dsl SINUMERIK Operate
Section 5
Measuring workpiece
Notes 5.5
Workpiece zero measure "Rectangular spigot"
The workpiece is parallel to the coordinate system on the work table and is a rectangle. About 4 measuring points of the center of the rectangle is determined. The following requirements must be met: Any tool can be used for scratching when loaded into the spindle for workpiece zero manual measuring. An electronic workpiece probe when loaded into the spindle and activated will measure the workpiece zero automatically. Pressing the VSK 6 "Rectangular spigot" softkey in the function "Meas. Workp. " (" Machine "in the" JOG ") appears on the screen the following input mask.
5.5.1 Vertical softkey bar (VSK) See page 20, Measure workpiece "Set edge".
5.5.2 Parameter Measure workpiece "Rectangular spigot" The following parameters of Measure workpiece "Set edge" are also at work measure "Rectangular spigot": [Zero offset G54, X0, Y0]
828D/840Dsl SINUMERIK Operate
Page 21
M570
Section 6 Notes
Measure tool 6.1
Selecting the function “Measure tool“
The geometries of the machining tool must be taken into consideration when executing a part program. These are stored as tool offset data in the tool list. Each time the tool is called, the control considers the tool offset data. When programming the part program, you only need to enter the workpiece dimensions from the production drawing. After this, the controller independently calculates the individual tool path. You can determine the tool offset data, i.e. the length and radius or diameter, either manually or automatically with tool probes. By pressing the HSK 4 “Meas. tool“ in the operating mode “JOG” under the operating area “Machine” the following window opens:
Measuring a tool manually For manual measurement, move the tool manually to a known reference point to determine the tool length and the radius or diameter. The control then calculates the tool offset data from the position of the tool carrier reference point and the reference point. With the measuring of the tool length either the workpiece or a fixed point in the machines coordinate system, e.g. a load cell or a fixed point in conjunction with a distance meter, can be used as a reference point. The position of the workpiece is specified during the measurement. The position of the fixed point however must be announced before the measurement. With the determination of the radius or diameter the workpiece always serves as the reference point. Hint: Depending on the setting in a machine data either the radius or the diameter of the tool can be measured. Note: Refer to the machine manufacturer's specifications.
M570
Page 22
828D/840Dsl SINUMERIK Operate
Section 6
Measure tool 6.2
Notes
Vertical softkey bar (VSK)
Display area
Description By pressing the VSK 1 ”Length manual” the “Length manual” input mask opens. By pressing the VSK 2 “Radius manual“ or rather “Diameter manual“ the input mask “Radius manual“ or rather “Diameter manual“ opens.
By pressing the VSK 7 ”Calibrate fixed pt.” the “Calibrate: fixed point” input mask opens. By pressing the VSK 8 “Back“ you jump back to the “Meas. tool” screen of the Sinumerik Operate.
828D/840Dsl SINUMERIK Operate
Page 23
M570
Section 6 Notes
Measure tool 6.3
Measure tool “Length manual” By pressing the HSK 4 “Meas. tool” and the VSK 1 “Length manual“ (in the operating area “Machine“ under the operating mode “JOG”) the following input mask opens.
6.3.1 Vertical softkey bar (VSK) Display area
Description By pressing the VSK 2 “Tool“ the tool list opens. See module M573 - “Operating area Parameter“. By pressing the VSK 7 “Set length“ the entered values will be accepted. By pressing the VSK 8 “Back“ you jump back to the “Measure tool” screen of the Sinumerik Operate.
M570
Page 24
828D/840Dsl SINUMERIK Operate
Section 6
Measure tool 6.3.2 Parameters of measure tool “Length manual“ Parameter
Description
T
Tool name Alternatively you can select a tool via the VSK 1 “Select tool”.
D
Edge number (1 to 9)
ST
Replacement tool (01- 99)
Ref. point
Workpiece or Fixed pt.
Z0
Workpiece edge
Notes
6.3.3 Procedure for Measuring tool “Length manual” 1.
Load the tool in the spindle you want to measure.
2.
In the operating mode “JOG“ press the HSK 4 “Meas. tool”.
3.
Press the VSK 1 “Length manual”. The “Length manual” input screen opens.
4.
Press the VSK 2 “Tool“. Select a tool from the “Tool list” that opens immediately after pressing the softkey.
5
Press the VSK 1 „In manual“ to switch back with the selected tool to the “Length manual” window.
4.
Select the cutting edge number “D” and the number of the replacement tool “ST”.
5.
Approach the workpiece in the Z direction, scratch it with a rotating spindle
6.
Enter the set position “Z0” of the workpiece edge.
7.
Press the VSK "Set length" softkey.
The tool length is calculated automatically and entered in the tool list.
828D/840Dsl SINUMERIK Operate
Page 25
M570
Section 6 Notes
Measure tool 6.4
Measure tool ”Radius manual“ or “Diameter manual” By pressing the HSK 4 “Meas. tool” and the VSK 2 “Radius manual“ or “Diameter manual” (in the operating area “Machine“ and operating mode “JOG”) the following input mask opens.
6.4.1 Vertical Softkey bar (VSK) Display area
Description By pressing the VSK 2 “Select tool” the tool list opens. By pressing the VSK 7 “Set diamet.“ (or “Set radius.”) all entered values will be accepted. By pressing the VSK 8 “Back“ you jump back to the “Measure tool” screen of the Sinumerik Operate“.
6.4.2 Parameters measure tool “Radius manual“ or “Diameter manual” The following parameters of the function “Length manual” are used also with “Radius manual” and “Diameter manual”: [T, D, ST] Beside the before mentioned parameters you find the following additional parameters in the “Radius manual” or “Diameter manual” window:
M570
Parameter
Description
X0
Workpiece edge
Y0
Workpiece edge Page 26
828D/840Dsl SINUMERIK Operate
Section 6
Measure tool 6.4.3 Procedure for measuring the tool “radius manual” (or “diameter manual” ) 1.
Load the tool you want to measure in the spindle.
2.
In the operating mode “JOG“ and operating area “Machine” press the HSK 4 “Meas. tool“.
3.
Press the VSK 2 “Radius manual“ ( or “Diameter manual“).
4.
Select the cutting edge number “D” and the number of the replacement tool “ST” of the tool.
5.
Approach the workpiece in the X- or Y-direction and perform scratching with the spindle rotating in the opposite direction.
6.
Specify the setpoint position “X0” or “Y0” of the workpiece edge.
7.
Press the "Set radius" or "Set diameter" softkey.
Notes
The tool radius or diameter is calculated automatically and entered in the tool list.
828D/840Dsl SINUMERIK Operate
Page 27
M570
Section 6 Notes
Measure tool 6.5
Selecting the function “Calibrate fixed point”
If you want to measure your tools manually, you must first determine the height of the fixed point on the machine table with reference to the machine zero. The fixed point can be either a measuring gauge of a known height or an electronic height gauge of known height. Place the gauge in the working area of the machine (e.g on the machine table) and align it relative to the machining axes. You can use any type of tool to measure the fixed point. You must enter the length and radius/diameter of the tool in the tool list beforehand. Note: Refer to the machine manufacturer's specifications.
By pressing the HSK 4 “Meas. tool” and the VSK 7 “Calibrate fixed pt.“ (in the operating area “Machine“ and operating mode “JOG”) the “Fixed point calibration” window opens.
M570
Page 28
828D/840Dsl SINUMERIK Operate
Section 6
Measure a tool
Notes
6.5.1 Vertical softkey bar (VSK) Display area
Description By pressing the VSK 7 “Calibrate“ the control calculates the fixed point height. By pressing the VSK 8 “Back“ you switch back to the “Measure tool” window.
6.5.2 Parameters of measure tool “Calibrate: fixed height” By calibrating the probe the following parameters are displayed: Parameter
Unit
Description
DZ
[mm]
Is the distance from the table to top of the fixed point gauge.
6.5.3 procedure for tool measure “Calibrating fixed point” 1.
Move the calibration tool until it is approximately over the centre of the measuring surface of the fixed point gauge
2.
In the operating mode “JOG“ press the HSK 4 “Meas. tool“.
3.
Press the VSK 6 “Calibrate fixed pt.”.
4.
Use the JOG keys in “Incremental mode, or the handwheel to position the tool at the fixed position height.
5.
Press the “Calibrate“ softkey to calibrate the fixed point.
828D/840Dsl SINUMERIK Operate
Page 29
M570
Section 7 Notes
Position 7.1
Selecting the function “Position“
In order to implement simple machining sequences, you can traverse the axes to certain positions in manual mode. Note: The feedrate/rapid traverse override is active during traversing. By pressing the HSK 6 “Position” in the Operating area “Machine” and operating mode “JOG” the following input mask will be shown on the screen:
7.2
Vertical softkey bar (VSK)
Display area
Description By pressing the VSK 5 “Rapid” the value of the set machine data for feed rate velocity in JOG is taken over in the parameter “F” (feed). Hint: The VSK 5 “Rapid traverse” can also be pressed if the input field parameter “F” is not the active input field (highlighted in orange) By pressing the VSK 8 “Back” you switch back to the main screen of the Sinumerik Operate.
M570
Page 30
828D/840Dsl SINUMERIK Operate
Section 7
Position 7.3
Notes
Parameters of “Position”
Parameter
Unit
Description
F
[mm/min] [mm/tooth]
Feed
X
[mm]
Target position of the selected axes [abs/inc]
Y Note: Several target positions can be entered. B-axis and C-axis are manufacturer specific. Follow the documentation of the machine manufacturer.
Z
SP
[Degree]
Target angle [abs, inc]
7.4. Procedure for positioning the axes 1.
Select the “JOG” operating mode.
2.
Press the HSK 6 “Position”.
3.
Specify the desired value for the feedrate “F”. - OR -
3.
Press VSK 5 "Rapid". *Rapid tr.* is displayed in the input field “F”.
4.
Enter the target position or the target angle for the axis or axes to be traversed.
5.
Press the "CYCLE START" button on the machine control panel. The axis is traversed to the specified target position.
Note: If target positions were specified for several axes, the axes are traversed simultaneously.
828D/840Dsl SINUMERIK Operate
Page 31
M570
Section 8 Notes
Face milling 8.1
Selecting the function “Face milling”
You can use this cycle to face mill any workpiece. A rectangular surface is always machined. “Measuring the workpiece" is already mentioned in section 5. The input mask “Face milling” is described in relation to a workpiece with dimensions 25x100x100 mm, with 1mm to be removed leaving a thickness of 24mm.
The zero point in the X and Y axis has been determined in the workpiece center with measuring function "Rectangular spigot" and the Z axis was "set edge" with Z value +1 mm determined and stored at zero 1 (G54).
By pressing the HSK 7 “Face mill.” in the Operating area “Machine” and operating mode “JOG” the following input mask will be shown on the screen.
M570
Page 32
828D/840Dsl SINUMERIK Operate
Section 8
Face milling
Notes 8.2
Vertical softkey bar (VSK)
Display area
Description By pressing the VSK 1 „Select tool“ you can insert a tool. Select the desired tool in the tool list (e.g FACEMILL_50 with the orange selection cursor and press VSK 1 “In program” With VSK 2 ”Graphic view” you can switchover between help screen and graphical view. With VSK 3 "lateral limitation left" you can specify the lateral limitation in “X-” direction. With VSK 4 "lateral limitation top" you can specify the lateral limitation in “Y+” direction. With VSK 5 "lateral limitation right" you can specify the lateral limitation in “X+” direction. With VSK 6 "lateral limitation bottom" you can specify the lateral limitation in “Y-” direction. By pressing the VSK 7 “Cancel” you can escape the screen “face milling”. With pressing of VSK 8 ”Accept” the following program block is generated:
With “CYCLE START“ the cycle “Face milling” will be executed.
828D/840Dsl SINUMERIK Operate
Page 33
M570
Section 8 Notes
Face milling 8.3
Parameters of “Face milling”
Parameter
Unit
Description
T
Tool name
D
Cutting edge number of the tool.
F
[mm/min] Feed [mm/tooth]
S V
[rpm] [m/min]
Machining
Spindle speed or constant cutting speed The following machining operations can be selected: Roughing Finishing
Direction Same direction of machining Alternating direction of machining
M570
X0 Y0 Z0
mm
Corner point 1 of surface in X direction (abs) Corner point 1 of surface in Y direction (abs) Height of blank (abs)
X1 Y1 Z1
mm
Corner point 2 of surface in X (abs or inc) Corner point 2 of surface in Y (abs or inc) Height of finished part (abs or inc)
DXY
mm %
Max. infeed in the XY plane (dependent on milling cutter diameter) Alternatively you can specify the plane infeed as a %, as a ratio plane infeed (mm) to milling cutter diameter (mm).
DZ
mm
Max. infeed in Z direction (only for roughing)
UZ
mm
Finishing allowance, depth
Page 34
828D/840Dsl SINUMERIK Operate
Section 9
Settings 9.1
Notes
Selecting the function “Settings”
You can predefine millimetre or inch as the measuring units for the control unit. The change-over of the measurement units is done for the whole control. All necessary entries are thereby converted automatically into the new measurement units, e.g.: Positional data Tool corrections Zero point offsets By pressing the HSK 2.8 “Settings” in the extended horizontal softkey bar in operation area “Machine” under operation mode “JOG” the following input mask will be shown on the screen.
9.2
Vertical softkey bar (VSK)
Display area
Description By pressing the VSK 5 "Changeover inch" the measuring units are converted from the metric to the imperial (inch) dimension system. New values have to be entered in inches. By pressing this key the key function switches to "Changeover metric". By pressing the VSK 5 "Changeover metric" the measuring units are converted from the imperial (inch) to the metric dimension system. New values have to be metric. By pressing this key the key function switches to "Changeover inch". Accept the selection by pressing the VSK 8 “OK” or cancel by pressing the VSK 7 “Cancel”. By pressing the VSK 8 "Back" you switch back to the main screen of the Sinumerik Operate with extended HSK.
828D/840Dsl SINUMERIK Operate
Page 35
M570
Section 9
Settings
Notes 9.3
Measurement units [metric/imperial]
Country specific settings of the measuring units are not displayed in the input masks. In the following table the measuring units metric and imperial are compared with one another. A switchover can be made in the "T,S,M," input mask or by pressing the HSK 2.8 “Settings” in the extended HSK-bar and VSK 5 “Changeover Inch” or “Changeover Metric” as mentioned before. metric
Inch
mm
in
mm/tooth
in/tooth
mm/min
in/min
mm/U
in/U
m/min
ft/min
9.4
Parameter setting for manual operation
In the “Settings for manual mode“ window all configurations for manual operation can be done. Parameter
Unit
Meaning
Type of feedrate: G94 G95
[mm/min] [mm/rev]
Axis feedrate/linear feedrate Revolutional feedrate
[mm/min] [mm/rev]
Axis feedrate/linear feedrate Revolutional feedrate
Setup feedrate: G94 G95 Variable increment
Spindle speed
Enter the desired increment for axis traversal by variable increments [rpm]
Spindle speed in revolutions per minute
After inserting the values in the input fields, press the VSK 8 “Back“ to switch back to the main screen of the Sinumerik Operate in the extended view.
M570
Page 36
828D/840Dsl SINUMERIK Operate
