suzanne.soy/FreeCAD
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

Added contributed post-processor scripts.

Browse Source
This commit is contained in:
ml 2016-10-23 01:40:02 -07:00 committed by wmayer
parent 98e93d329f
commit 3d3a63deaf
2 changed files with 686 additions and 0 deletions
Show Stats Download Patch File Download Diff File Expand all files Collapse all files

266
src/Mod/Path/PathScripts/dynapath_post.py Normal file
View File

@ -0,0 +1,266 @@
#***************************************************************************
#* (c) sliptonic (shopinthewoods@gmail.com) 2014 *
#* *
#* This file is part of the FreeCAD CAx development system. *
#* *
#* This program is free software; you can redistribute it and/or modify *
#* it under the terms of the GNU Lesser General Public License (LGPL) *
#* as published by the Free Software Foundation; either version 2 of *
#* the License, or (at your option) any later version. *
#* for detail see the LICENCE text file. *
#* *
#* FreeCAD is distributed in the hope that it will be useful, *
#* but WITHOUT ANY WARRANTY; without even the implied warranty of *
#* MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the *
#* GNU Lesser General Public License for more details. *
#* *
#* You should have received a copy of the GNU Library General Public *
#* License along with FreeCAD; if not, write to the Free Software *
#* Foundation, Inc., 59 Temple Place, Suite 330, Boston, MA 02111-1307 *
#* USA *
#* *
#* This file has been modified from Sliptonis original Linux CNC post *
#* for use with a Dynapath 20 controller all changes and Modifications *
#* (c) Linden (Linden@aktfast.net) 2016 *
#* *
#***************************************************************************/
TOOLTIP='''
This is a postprocessor file for the Path workbench. It is used to
take a pseudo-gcode fragment outputted by a Path object, and output
real GCode suitable for a Tree Journyman 325 3 axis mill with Dynapath 20 controller in MM.
This is a work in progress and very few of the functions available on the Dynapath have been
implemented at this time.
This postprocessor, once placed in the appropriate PathScripts folder, can be used directly
from inside FreeCAD, via the GUI importer or via python scripts with:
Done
Coordinate Decimal limited to 3 places
Feed limited to hole number no decimal
Speed Limited to hole number no decimal
Machine Travel Limits Set to approximate values
Line numbers start at one and incremental by 1
Set preamble
Set postamble
To Do
Change G20 and G21 to G70 and G71 for metric or imperial units
Convert arcs to absolute
Strip comments and white spaces
Add file name in brackets limited to 8 alpha numeric no spaces all caps as first line in file
Change Q to K For depth of peck on G83
Fix tool change
Limit comments length and characters to Uppercase, alpha numeric and spaces add / prior to coments
import linuxcnc_post
linuxcnc_post.export(object,"/path/to/file.ncc")
'''
import datetime
now = datetime.datetime.now()
from PathScripts import PostUtils
#These globals set common customization preferences
OUTPUT_COMMENTS = True
OUTPUT_HEADER = False
OUTPUT_LINE_NUMBERS = False
SHOW_EDITOR = True
MODAL = False #if true commands are suppressed if the same as previous line.
COMMAND_SPACE = " "
LINENR = 1 #line number starting value
#These globals will be reflected in the Machine configuration of the project
UNITS = "G21" #G21 for metric, G20 for us standard
MACHINE_NAME = "Tree MM"
CORNER_MIN = {'x':-340, 'y':0, 'z':0 }
CORNER_MAX = {'x':340, 'y':-355, 'z':-150 }
#Preamble text will appear at the beginning of the GCODE output file.
PREAMBLE = '''G17
G90
;G90.1 ;needed for simulation only
G80
G40
'''
#Postamble text will appear following the last operation.
POSTAMBLE = '''M09
M05
G80
G40
G17
G90
M30
'''
#Pre operation text will be inserted before every operation
PRE_OPERATION = ''''''
#Post operation text will be inserted after every operation
POST_OPERATION = ''''''
#Tool Change commands will be inserted before a tool change
TOOL_CHANGE = ''''''
# to distinguish python built-in open function from the one declared below
if open.__module__ == '__builtin__':
pythonopen = open
def export(objectslist,filename):
global UNITS
for obj in objectslist:
if not hasattr(obj,"Path"):
print "the object " + obj.Name + " is not a path. Please select only path and Compounds."
return
print "postprocessing..."
gcode = ""
#Find the machine.
#The user my have overriden post processor defaults in the GUI. Make sure we're using the current values in the Machine Def.
myMachine = None
for pathobj in objectslist:
if hasattr(pathobj,"Group"): #We have a compound or project.
for p in pathobj.Group:
if p.Name == "Machine":
myMachine = p
if myMachine is None:
print "No machine found in this project"
else:
if myMachine.MachineUnits == "Metric":
UNITS = "G21"
else:
UNITS = "G20"
# write header
if OUTPUT_HEADER:
gcode += linenumber() + "(Exported by FreeCAD)\n"
gcode += linenumber() + "(Post Processor: " + __name__ +")\n"
gcode += linenumber() + "(Output Time:"+str(now)+")\n"
#Write the preamble
if OUTPUT_COMMENTS: gcode += linenumber() + "(begin preamble)\n"
for line in PREAMBLE.splitlines(True):
gcode += linenumber() + line
gcode += linenumber() + UNITS + "\n"
for obj in objectslist:
#do the pre_op
if OUTPUT_COMMENTS: gcode += linenumber() + "(begin operation: " + obj.Label + ")\n"
for line in PRE_OPERATION.splitlines(True):
gcode += linenumber() + line
gcode += parse(obj)
#do the post_op
if OUTPUT_COMMENTS: gcode += linenumber() + "(finish operation: " + obj.Label + ")\n"
for line in POST_OPERATION.splitlines(True):
gcode += linenumber() + line
#do the post_amble
if OUTPUT_COMMENTS: gcode += "(begin postamble)\n"
for line in POSTAMBLE.splitlines(True):
gcode += linenumber() + line
if SHOW_EDITOR:
dia = PostUtils.GCodeEditorDialog()
dia.editor.setText(gcode)
result = dia.exec_()
if result:
final = dia.editor.toPlainText()
else:
final = gcode
else:
final = gcode
print "done postprocessing."
gfile = pythonopen(filename,"wb")
gfile.write(gcode)
gfile.close()
def linenumber():
global LINENR
if OUTPUT_LINE_NUMBERS == True:
LINENR += 1
return "N" + str(LINENR) + " "
return ""
def parse(pathobj):
out = ""
lastcommand = None
#params = ['X','Y','Z','A','B','I','J','K','F','S'] #This list control the order of parameters
params = ['X','Y','Z','A','B','I','J','F','S','T','Q','R','L'] #linuxcnc doesn't want K properties on XY plane Arcs need work.
if hasattr(pathobj,"Group"): #We have a compound or project.
if OUTPUT_COMMENTS: out += linenumber() + "(compound: " + pathobj.Label + ")\n"
for p in pathobj.Group:
out += parse(p)
return out
else: #parsing simple path
if not hasattr(pathobj,"Path"): #groups might contain non-path things like stock.
return out
if OUTPUT_COMMENTS: out += linenumber() + "(Path: " + pathobj.Label + ")\n"
for c in pathobj.Path.Commands:
outstring = []
command = c.Name
outstring.append(command)
# if modal: only print the command if it is not the same as the last one
if MODAL == True:
if command == lastcommand:
outstring.pop(0)
# Now add the remaining parameters in order
for param in params:
if param in c.Parameters:
if param == 'F':
outstring.append(param + format(c.Parameters['F'], '.0f'))
elif param == 'S':
outstring.append(param + format(c.Parameters[param], '.0f'))
elif param == 'T':
outstring.append(param + format(c.Parameters['T'], '.0f'))
else:
outstring.append(param + format(c.Parameters[param], '.3f'))
# store the latest command
lastcommand = command
# Check for Tool Change:
if command == 'M6':
if OUTPUT_COMMENTS: out += linenumber() + "(begin toolchange)\n"
for line in TOOL_CHANGE.splitlines(True):
out += linenumber() + line
if command == "message":
if OUTPUT_COMMENTS == False:
out = []
else:
outstring.pop(0) #remove the command
#prepend a line number and append a newline
if len(outstring) >= 1:
if OUTPUT_LINE_NUMBERS:
outstring.insert(0,(linenumber()))
#append the line to the final output
for w in outstring:
out += w + COMMAND_SPACE
out = out.strip() + "\n"
return out
print __name__ + " gcode postprocessor loaded."

420
src/Mod/Path/PathScripts/generic_post.py Normal file
View File

@ -0,0 +1,420 @@
# -*- coding: utf-8 -*-
#***************************************************************************
#* *
#* Copyright (c) 2016 Christoph Blaue <blaue@fh-westkueste.de> *
#* *
#* This program is free software; you can redistribute it and/or modify *
#* it under the terms of the GNU Lesser General Public License (LGPL) *
#* as published by the Free Software Foundation; either version 2 of *
#* the License, or (at your option) any later version. *
#* for detail see the LICENCE text file. *
#* *
#* This program is distributed in the hope that it will be useful, *
#* but WITHOUT ANY WARRANTY; without even the implied warranty of *
#* MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the *
#* GNU Library General Public License for more details. *
#* *
#* You should have received a copy of the GNU Library General Public *
#* License along with this program; if not, write to the Free Software *
#* Foundation, Inc., 59 Temple Place, Suite 330, Boston, MA 02111-1307 *
#* USA *
#* *
#***************************************************************************
TOOLTIP='''Post processor for Maho M 600E mill
Machines with Philips or Heidenhain control should be very easy to adapt.
The post processor is configurable by changing the values of constants.
No programming experience required. This can make a generated g-code
program more readable and since older machines have very
limited memory it seems sensible to reduce the number of commands and
parameters, like e.g. suppress the units in the header and at every hop.
'''
# reload in python console:
# import maho_post
# reload(maho_post)
import FreeCAD
import time
import Path, PathScripts
from PathScripts import PostUtils
import math
#***************************************************************************
# user editable stuff here
MACHINE_NAME = 'Maho 600E'
CORNER_MIN = {'x':-51.877, 'y':0, 'z':0 } #use metric for internal units
CORNER_MAX = {'x':591.5, 'y':391.498, 'z':391.5 } #use metric for internal units
UNITS = 'G21' # use metric units
# possible values:
# 'G20' for inches,
# 'G21' for metric units.
# a mapping to different GCodes is handled in the GCODE MAP below
UNITS_INCLUDED = False # do not include the units in the GCode program
# possible values:
# True if units should be included
# False if units should not be included
# usually the units to be used are defined in the machine constants and almost never change,
# so this can be set to False.
COMMENT = ''
# possible values:
# ';' centroid or sinumerik comment symbol,
# '' leave blank for bracketed comments style "(comment comment comment)"
# '...' any other symbol to start comments
# currently this can be only one symbol, if it should be a sequence of characters
# in PostUtils.py the line
# if len(commentsym)==1:
# should be changed to
# if len(commentsym)>1:
SHOW_EDITOR = True
# possible values:
# True before the file is written it is shown to the user for inspection
# False the file is written directly
LINENUMBERS = True
# possible values:
# True if linenumbers of the form N1 N2 ... should be included
# False linennumbers are suppressed
# if linenumbers are used, header and footer get numbered as well
STARTLINENR = 1 # first linenumber used
# possible values:
# any integer value >= 0
# to have the possibility to change some initial values directly at the CNC machine
# without renumbering the rest it is possible to start the numbering of the file with some value > 0
LINENUMBER_INCREMENT = 1
# possible values:
# any integer value > 0
# similar to STARTLINENR it is possible to leave gaps in the linenumbering of subsequent lines
MODAL = True
# possible values:
# True repeated GCodes in subsequent lines are suppressed, like in the following snippet
# G1 X10 Y20
# X10 Y30
# False repeated GCodes in subsequent lines are repeated in the GCode file
# G1 X10 Y20
# G1 X10 Y30
MODALPARAMS = ['X','Y','Z','S','F'] # suppress these parameters if they haven't changed
# possible values:
# any list of GCode parameters
# if a parameter doesn't change from one line to the next ( or even further) it is suppressed.
# Example:
# G1 X10 Y20
# G1 Y30
# If in addition MODAL is set to True, the generated GCode changes to
# G1 X10 Y20
# Y30
SWAP_G2_G3 = True # some machines have the sign of the X-axis swapped, so they behave like milling from the bottom
# possible values:
# True if left and right turns are to be swapped
# False don't swap
# this might be special with some maho machines or even with mine and might be changed in the machine constants as well
SWAP_Y_Z = True # machines with an angle milling head do not switch axes, so we do it here
# possible values:
# True if Y and Z values have to be swapped
# False do not swap
# For vertical milling machines the Z-axis is horizontal (of course).
# If they have an angle milling head, they mill vertical, alas the Z-axis stays horizontal.
# With this parameter we can swap the output values of Y and Z.
# For commands G2 and G3 this means that J and K are swapped as well
ABSOLUTE_CIRCLE_CENTER = True
# possible values:
# True use absolute values for the circle center in commands G2, G3
# False values for I, J, K are given relative to the last point
USE_RADIUS_IF_POSSIBLE = True
# possible values:
# True if in commands G2 and G3 the usage of radius R is preferred
# False if in commands G2 and G3 we use always I and J
# When milling arcs there are two reasons to use the radius instead of the center:
# 1. the GCode program might be easier to understand
# 2. Some machines seem to have a different scheme for calculating / rounding the values of the center
# Thus it is possible that the machine complains, that the endpoint of the arc does not lie on the arc.
# Using the radius instead avoids this problem.
# The post processor takes care of the fact, that only angles <= 180 degrees can be used with R
# for larger angles the center is used independent of the setting of this constant
RADIUS_COMMENT = True
# possible values:
# True for better understanding the radius of an arc is included as a comment
# False no additional comment is included
# In case the comments are included they are always included with the bracketing syntax like '(R20.456)'
# and never with the comment symbol, because the radius might appear in the middle of a line.
GCODE_MAP = {'M1':'M0', 'M6':'M66', 'G20':'G70', 'G21':'G71'} # cb: this could be used to swap G2/G3
# possible values:
# Comma separated list of values of the form 'sourceGCode':'targetGCode'
#
# Although the basic movement commands G0, G1, G2 seem to be used uniformly in different GCode dialects,
# this is not the case for all commands.
# E.g the Maho dialect uses G70 and G71 for the units inches vs. metric.
# The map {'M1':'M0', 'G20':'G70', 'G21':'G71'} maps the optional stop command M1 to M0,
# because some Maho machines do not have the optional button on its panel
# in addition it maps inches G20 to G70 and metric G21 to G71
AXIS_DECIMALS = 3
# possible values:
# integer >= 0
FEED_DECIMALS = 2
# possible values:
# integer >= 0
SPINDLE_DECIMALS = 0
# possible values:
# integer >= 0
# The header is divided into two parts, one is dynamic, the other is a static GCode header.
# If the current selection and the current time should be included in the header,
# it has to be generated at execution time, and thus it cannot be held in constant values.
# The last linefeed should be ommitted, it is inserted automatically
# linenumbers are inserted automatically if LINENUMBERS is True
# if you don't want to use this header you have to provide a minimal function
# def mkHeader(selection):
# return ''
def mkHeader(selection):
# this is within a function, because otherwise filename and time don't change when changing the FreeCAD project
# now = datetime.datetime.now()
now = time.strftime("%Y-%m-%d %H:%M")
originfile = FreeCAD.ActiveDocument.FileName
headerNoNumber = "%PM\n" # this line gets no linenumber
headerNoNumber += "N9XXX (" + selection[0].Description + ", " + now + ")\n" # this line gets no linenumber, it is already a specially numbered
header = ""
# header += "(Output Time:" + str(now) + ")\n"
header += "(" + originfile + ")\n"
header += "(Exported by FreeCAD)\n"
header += "(Post Processor: " + __name__ +")\n"
header += "(Target machine: " + MACHINE_NAME + ")"
return headerNoNumber + linenumberify(header)
GCODE_HEADER = "" # do not terminate with a newline, it is inserted by linenumberify
#GCODE_HEADER = "G40 G90" # do not terminate with a newline, it is inserted by linenumberify
#possible values:
# any sequence of GCode, multiple lines are welcome
# this constant header follows the text generated by the function mkheader
# linenumbers are inserted automatically if LINENUMBERS is True
GCODE_FOOTER = "M30" # do not terminate with a newline, it is inserted by linenumberify
#possible values:
# any sequence of GCode, multiple lines are welcome
# the footer is used to clean things up, reset modal commands and stop the machine
# linenumbers are inserted automatically if LINENUMBERS is True
# don't edit with the stuff below the next line unless you know what you're doing :)
#***************************************************************************
linenr = 0 # variable has to be global because it is used by linenumberify and export
if open.__module__ == '__builtin__':
pythonopen = open
def angleUnder180(command,lastX,lastY,x,y,i,j):
# radius R can be used iff angle is < 180.
# This is the case
# if the previous point is left of the current and the center is below (or on) the connection line
# or if the previous point is right of the current and the center is above (or on) the connection line
middleOfLineY = (lastY + y)/2
centerY = lastY + j
if ((command == 'G2' and ( (lastX == x and ((lastY<y and i>=0) or (lastY > y and i <= 0))) or (lastX < x and centerY <= middleOfLineY) or (lastX > x and centerY >= middleOfLineY)))
or (command == 'G3' and ((lastX == x and ((lastY<y and i<=0) or (lastY > y and i >= 0))) or (lastX < x and centerY >= middleOfLineY) or (lastX > x and centerY <= middleOfLineY)))):
return True
else:
return False
def mapGCode(command):
if command in GCODE_MAP:
mappedCommand = GCODE_MAP[command]
else:
mappedCommand = command
if SWAP_G2_G3:
if command == 'G2':
mappedCommand = 'G3'
elif command == 'G3':
mappedCommand = 'G2'
return mappedCommand
def linenumberify(GCodeString):
# add a linenumber at every beginning of line
global linenr
if not LINENUMBERS:
result = GCodeString + "\n"
else:
result = '';
strList = GCodeString.split("\n")
for s in strList:
if s:
# only non empty lines get numbered. the special lines "%PM" and prognumber "N9XXX" are skipped
result += "N" + str(linenr) + " " + s + "\n"
linenr += LINENUMBER_INCREMENT
else:
result += s + "\n"
return result
def export(selection,filename):
global linenr
linenr = STARTLINENR
lastX = 0
lastY = 0
lastZ = 0
params = ['X','Y','Z','A','B','I','J','F','H','S','T','Q','R','L'] #Using XY plane most of the time so skipping K
modalParamsDict = dict()
for mp in MODALPARAMS:
modalParamsDict[mp] = None
for obj in selection:
if not hasattr(obj,"Path"):
print "the object " + obj.Name + " is not a path. Please select only path and Compounds."
return
myMachine = None
for pathobj in selection:
if hasattr(pathobj,"Group"): #We have a compound or selection.
for p in pathobj.Group:
if p.Name == "Machine":
myMachine = p
if myMachine is None:
print "No machine found in this selection"
else:
if myMachine.MachineUnits == "Metric":
UNITS = "G21"
else:
UNITS = "G20"
gcode =''
gcode+= mkHeader(selection)
gcode+= linenumberify(GCODE_HEADER)
if UNITS_INCLUDED:
gcode += linenumberify(mapGCode(UNITS))
lastcommand = None
gobjects = []
for g in selection[0].Group:
if g.Name <>'Machine': #filtering out gcode home position from Machine object
gobjects.append(g)
for obj in gobjects:
if hasattr(obj,'GComment'):
gcode += linenumberify('(' + obj.GComment + ')')
for c in obj.Path.Commands:
outstring = []
command = c.Name
if (command != UNITS or UNITS_INCLUDED):
if command[0]=='(':
command = PostUtils.fcoms(command, COMMENT)
mappedCommand = mapGCode(command) # the mapping is done for output only! For internal things we still use the old value.
if not MODAL or command != lastcommand:
outstring.append(mappedCommand)
# if MODAL == True: )
# #\better: append iff MODAL == False )
# if command == lastcommand: )
# outstring.pop(0!#\ )
if c.Parameters >= 1:
for param in params:
if param in c.Parameters:
if (param in MODALPARAMS) and (modalParamsDict[str(param)] == c.Parameters[str(param)]):
# do nothing or append white space
outstring.append(' ')
elif param == 'F':
outstring.append(param + PostUtils.fmt(c.Parameters['F'], FEED_DECIMALS,UNITS))
elif param == 'H':
outstring.append(param + str(int(c.Parameters['H'])))
elif param == 'S':
outstring.append(param + PostUtils.fmt(c.Parameters['S'], SPINDLE_DECIMALS,'G21')) #rpm is unitless-therefore I had to 'fake it out' by using metric units which don't get converted from entered value
elif param == 'T':
outstring.append(param + str(int(c.Parameters['T'])))
elif param == 'I' and (command == 'G2' or command == 'G3'):
# this is the special case for circular paths, where relative coordinates have to be changed to absolute
i = c.Parameters['I']
# calculate the radius r
j = c.Parameters['J']
r = math.sqrt(i**2 + j**2)
if USE_RADIUS_IF_POSSIBLE and angleUnder180(command,lastX,lastY,c.Parameters['X'],c.Parameters['Y'],i,j):
outstring.append('R' + PostUtils.fmt(r,AXIS_DECIMALS,UNITS))
else:
if RADIUS_COMMENT:
outstring.append('(R' + PostUtils.fmt(r,AXIS_DECIMALS,UNITS) + ')')
if ABSOLUTE_CIRCLE_CENTER:
i += lastX
outstring.append(param + PostUtils.fmt(i,AXIS_DECIMALS,UNITS))
elif param == 'J' and (command == 'G2' or command == 'G3'):
# this is the special case for circular paths, where incremental center has to be changed to absolute center
i = c.Parameters['I']
j = c.Parameters['J']
if USE_RADIUS_IF_POSSIBLE and angleUnder180(command,lastX,lastY,c.Parameters['X'],c.Parameters['Y'],i,j):
# R is handled with the I parameter, here: do nothing at all, keep the structure as with I command
pass
else:
if ABSOLUTE_CIRCLE_CENTER:
j += lastY
if SWAP_Y_Z:
# we have to swap j and k as well
outstring.append('K' + PostUtils.fmt(j,AXIS_DECIMALS,UNITS))
else:
outstring.append(param + PostUtils.fmt(j,AXIS_DECIMALS,UNITS))
elif param == 'K' and (command == 'G2' or command == 'G3'):
# this is the special case for circular paths, where incremental center has to be changed to absolute center
outstring.append('(' + param + PostUtils.fmt(c.Parameters[param],AXIS_DECIMALS,UNITS) + ')')
z = c.Parameters['Z']
k = c.Parameters['K']
if USE_RADIUS_IF_POSSIBLE and angleUnder180(command,lastX,lastY,c.Parameters['X'],c.Parameters['Y'],i,j):
# R is handled with the I parameter, here: do nothing at all, keep the structure as with I command
pass
else:
if ABSOLUTE_CIRCLE_CENTER:
k += lastZ
if SWAP_Y_Z:
# we have to swap j and k as well
outstring.append('J' + PostUtils.fmt(j,AXIS_DECIMALS,UNITS))
else:
outstring.append(param + PostUtils.fmt(j,AXIS_DECIMALS,UNITS))
elif param == 'Y' and SWAP_Y_Z:
outstring.append('Z' + PostUtils.fmt(c.Parameters[param],AXIS_DECIMALS,UNITS))
elif param == 'Z' and SWAP_Y_Z:
outstring.append('Y' + PostUtils.fmt(c.Parameters[param],AXIS_DECIMALS,UNITS))
else:
outstring.append(param + PostUtils.fmt(c.Parameters[param],AXIS_DECIMALS,UNITS))
if param in MODALPARAMS:
modalParamsDict[str(param)] = c.Parameters[param]
# save the last X, Y, Z values
if 'X' in c.Parameters:
lastX = c.Parameters['X']
if 'Y' in c.Parameters:
lastY = c.Parameters['Y']
if 'Z' in c.Parameters:
lastZ = c.Parameters['Z']
outstr = str(outstring)
outstr =outstr.replace(']','')
outstr =outstr.replace('[','')
outstr =outstr.replace("'",'')
outstr =outstr.replace(",",'')
if LINENUMBERS:
gcode += "N" + str(linenr) + " "
linenr += LINENUMBER_INCREMENT
gcode+= outstr + '\n'
lastcommand = c.Name
gcode+= linenumberify(GCODE_FOOTER)
if SHOW_EDITOR:
PostUtils.editor(gcode)
gfile = pythonopen(filename,"wb")
gfile.write(gcode)
gfile.close()