【原创】Post work with DMU-50,70, 50E, 70E 5 Axis Machine

以下是Run Post, 出NC程序給上述五軸機器的要點:
  
Working with the Postprocessor
  
Usually, there are two possibilities of machining with the postprocessor for DMU50/70:
- Working with G7/G141 or CYCL.19 M127/128
- Working without output of G7/G141 or CYCL.19 M127/128
  
Working with G7/G141 or CYCL.19 M127/128
  
The functions of G7 and CYCL.19 facilitate working on the machine for the operator. The NC programs
prepared are not created related to the tension orientation of the part towards the table centre. The control
calculates the relocation of the traverse path with internal functions for table turns in X, Y and Z. With this,
the programs are independent from the position of the part on the machine table!
The functions for G7 or CYCL.19 are set in the configuration mask of the postprocessors. When running
the postprocessor, no further relocations will be inputted. A zero point relocation will be invoked, in which
the programmed zero point of the part is inscribed.
  
NOTE!
With Heidenhain, the setting of the zero point is more complicated. In the machine constant, the zero point
can be output in the active zero point table additivly or based on the basing point of the machine. The
machine constant is set with the MOD key in the editing mode. After input of the key code 95148, MP7475
= 1 is set. Therefore, the zero point is related to the basing point of the machine. Be careful – in spite of
this, reference points that were set can change the zero point relocation. Therefore, you need to delete all
basing points.
  
Example:
0 BEGIN PGM TST MM
1 CYCL DEF 19.0 BEARBEITUNGSEBENE
2 CYCL DEF 19.1 A+0 B+0 C+0
3 CYCL DEF 19.0 BEARBEITUNGSEBENE
4 CYCL DEF 19.1
5 CYCL DEF 7.0 NULLPUNKT
6 CYCL DEF 7.1 #0
7 L M30
8 END PGM TST MM
  
Is the zero offset is additive, working with Heidenhain is very easy to disrupt.
Check the zero points frequently. In manual mode, move the machine to X0 Y0 and centre the spindle
towards the middle of the table.
  
On the MillPlus control, only zero point must to be set, e. g. with G54. This zero point must be invoked
during the postprocessor calculation run. This usually works on the first attempt.
  
Working without G7/G141 or CYCL.19 M127/128
  
If the functions of the postprocessor are deactivated, the postprocessor calculates the relocating of the
traverse path with table turns in X, Y and Z. For this, the position of the zero point of the part based on the
centre of the table must be known before running the calculation.
Proceed as follows:
1. Input of Parameter 13, 16, 19a and 19b from the Abnahmeprotokoll into the postprocessor.
2. Input of the table centre as zero offset, e. g. in G54 I50 (see following paragraph).
3. Alignment of the part in SURFCAM according to tension operation.
4. Setting of a zero point of the part (which is usually not identical with the table centre).
5. Programming of Surfcam with active construction views in construction coordinates.
6. Stretching of part on the table.
7. With active G54 (table centre = 0) move to the zero point of the part.
8. Input of the values shown in the display of control in X, Y, Z into the relocation of the postprocessor
calculation run. Do not set any new zero points or write over the zero point
9. Mill
10. The postprocessor calculation run must be done with new values, if tension towards the table centre is
changed.
  
Entering and Inspection of Machine Parameters
To enable a calculation for the tension orientation of the part towards the middle of the table, the values of
measurement will be entered from the Abnahmeprotokoll into machine constant by the manufacturer. The
values can be inspected as follows:
  
Heidenhain
  
See Heidenhain Documentation Chapter 14
Select one after the other:
Type of Operation: POSITIONING WITH MANUAL INPUT, READ IN PROGRAM, MOD
Input of key code 80766769 ENT
PGMMGT key for program management
In directory/Proto a file kine_1 with staus ME (which means table is active) is found.
Open ENT file to edit
   MP 7530  Abnahmeprotokoll Nr.              Distance to Reference Point
0 -250.762   13                                       X-Axis
1 -156.079   14                                       Y-Axis
2 -543.089   15                                       Z-Axis
3
4 -0.012    is calculated from (Nr 16 – Nr 13)/2
5 154.915    19b
  
For inspection, the traverse paths of the machine can be controlled in the machine constant.
MC 920.0 X-Axis
MC 920.1 Y-Axis
MC 920.2 Z-Axis
  
MillPlus
  
To work with G7/G141 the following entries in the machine constant are necessary:
Constant Abnahmeprotokoll No.
MC 603    13
MC 607    14
MC 611    15
MC 619    19b
MC 623    is calculated
  
For inspection, the traverse paths of the machine can be controlled in the machine constant:
MC 3114 X-Axis
MC 3214 Y-Axis
MC 3314 Z-Axis
  
Siemens
  
File Name:
TCA-DAT.SPF
Parameter 13, 14, 15, 16, 19b
  
For all controls, the following is applied at present:
Parameter 19a will not be included into the calculation, which could result into mistakes in the y-axis. If
this problem should appear at the customer‘ s, the machine should be programmed with the Syscam
Postprocessor without output of G7 or CYCL.19. The second axis offset is integrated into the
postprocessor and equals it by calculation.
  
Problems with Abnahmeprotokoll
  
The Abnahmeprotokoll unfortunately was not completed consistently according to the same rules.
Therefore, the following mistakes occured as described below:
Parameter 13, 14, 15, 16 were partly not measured on the of older machines. Since the display at Mill plus
did not control the distance to basing point, the positve rest traverse paths were partly entered into the
protocoll.
Note:
This mistake probably only appears in Mill Plus controls.
The values 13, 14, 15 and 16 must be negative!
Positive values point to a wrong output.
Inspection is very easy:
Mobe thehe machine related to reference point in x on value no. 13 and y on value no. 14. If the spindle is
not orientated on the middle of the table, take the traverse path in x and y from table below from 13 and
14. The result has to be negative! The machine is moved to these new values 13 and 14 and the spindle
is exactely on the middle of the table.
  
Example for Heidenhain:
1. Manually move the spindle left behind up until you reach end switch
2. Put x, y and z to zero
3. Switch to display of rest movement
4. LX-250.762 Y – 144.334 F MAX M91 (M91 is related to the basing point).
  
Example for MillPlus
1. N1 G74 X-250.762 Y –155.334
(G74 is related to the basing point and states speed movement).
  
Travers Path of the Particular Machines
  DMU50eV DMU50V DMU70V DMU70eV
X 500,6   500,6  710,6  750,6
Y 420,6   380,6  520,6  600,6
Z 380,6   380,6  520,6  520,6

由于工作需要，急需heidenhain的资料。不知哪位仁兄能帮我一下，传点过来，本人不胜感激！
E-mail:wd23961@sina.com

长见识