Denford triac question

[Yogesh K. Raman]

I had a educational client recently who requested that I do Mastercam on-site training in the shopfloor itself so that they can readily machine their projects they've done on the training.

 

To my suprise, a full program with a backplot simulation of 41 minutes took 4 hours to machine.... what went wrong? The machine was a denford triac CNC. Is there any way to get a more accurate estimate?

Thanks in advance.

[Eeyore-nonhuman forum member]

Yogesh !

 

Machines are different !

One has full G0 60m/min , some other may have

only 3 m/min .

One has huge data buffer and dataserver ,while some others can have buffer for 3 blocks (so it`s good idea to use filtering for toolpathes ,especially on slow machines )

Acceleration/decceleration may be different ,one can have acceleration up to 2-3 G ,other 10 times less

All this can influence the real part time .

That`s why during backplot you see the message that tool time is approxiamate and you need to use Setup sheet for correct time

if you look in notepad on some setup sheet file *.set you will see what to edit

~~~~~~~~~~~~~~~

# Post Name : MILLM.SET

# Product : MILL

# Machine Name : GENERIC

# Control Name : GENERIC

# Description : GENERIC SETUP SHEET FOR MILL VERSION 9 (Metric)

# Mill/Turn : NO

# 4-axis/Axis subs. : NO

# 5-axis : NO

# Executable : MP v9.10

#

# WARNING: THIS POST IS GENERIC AND IS INTENDED FOR MODIFICATION TO

# THE MACHINE TOOL REQUIREMENTS AND PERSONAL PREFERENCE.

#

# ---------------

#| REVISION LOG: |

# ------------------------------------------------------------------------

# Programmers Note:

# CNC 05/16/00 - Initial update for V8 (fixed preadbuf2)

# CNC 05/21/01 - Added Max/Min X,Y,Z axis output option.

# CNC 06/15/01 - Added tool information (mfg & chuck) outputs options.

# CNC 07/12/01 - Added Max/Min Feedrate output option (see Users Note).

# and Detailed Feed/Rapid time output option.

# CNC 07/17/01 - Added Stock Information output option (see Users Note).

# Added 'fs2' formats for Inch/Metric output.

# CNC 11/14/01 - Added additional Parameter (10000 type) info. retrieval.

# CNC 12/14/01 - Altered to use Rapid Feedrate setting from numbered questions.

# CNC 02/04/03 - Initial update for V9.1

#

# ---------------

#| FEATURES: |

# ------------------------------------------------------------------------

# Users Note -->>

#

#=============================================================================

# Specific setting to allow tuning the cycle time calculations ->

 

# Set the time it takes for machine to do a toolchange ->

tlchgtime : .1 # Tool Change Time (* in Minutes *)

 

# Set the Rapid Traverse Rate of the machine

38. Rapid feedrate (Inches per Minute)? 300.0

1538. Rapid feedrate (MM per Minute)? 10000.0

#These values are loaded into the pre-defined post variable -> pst_rpd_fr (v9)

 

#=============================================================================

# Post specific "switches" to allow turning ON/OFF the following functions ->

 

# X,Y,Z axis limits option switches...

# By setting the switch variables (to 'yes' or 'no') ->

# You can select which axis you wish to monitor.

X_limits : yes # Output MAX/MIN values for the X axis (yes/no)?

Y_limits : yes # Output MAX/MIN values for the Y axis (yes/no)?

Z_limits : yes # Output MAX/MIN values for the Z axis (yes/no)?

 

# The 'xyz_limits' switch allows selecting WHERE to output this information.

# Setting the 'xyz_limits' variable ->

#xyz_limits = 0, Do NOT output ANY Max/Min X,Y,Z information.

#xyz_limits = 1, Output Max/Min X,Y,Z info. ONLY for EACH tool (not Program)

#xyz_limits = 2, Output Max/Min X,Y,Z info. ONLY for entire Program

#xyz_limits = 3, Output Max/Min X,Y,Z info. for EACH tool AND Program

xyz_limits : 2 # Output Max/Min X,Y,Z information, where?

 

# The 'fr_limits' switch allows selecting WHERE to output the FEEDRATE MAX/MIN

# information.

# Setting the 'fr_limits' variable ->

#fr_limits = 0, Do NOT output ANY Max/Min Feedrate information.

#fr_limits = 1, Output Max/Min Feedrate info. ONLY for EACH tool (not Program)

#fr_limits = 2, Output Max/Min Feedrate info. ONLY at end for entire program

#fr_limits = 3, Output Max/Min Feedrate info. for EACH tool AND Program

fr_limits : 0 # Output Max/Min Feedrate information, where?

 

# The 'det_time' switch allows selecting the output of 'Detailed Times"

# In addition to the usual 'TOOL TIME', you can get the time spent at

# RAPID and at FEEDRATE during each tool and/or for the entire program.

# *IMPORTANT*

# Note that the Program TOTAL TIME includes the Toolchange time(s),

# so it will be longer than the Total RAPID time + Total FEED time!

#

# Setting the 'det_time' variable ->

#det_time = 0, Do NOT output ANY Rapid/Feedrate time breakdown.

#det_time = 1, Output Rapid/Feedrate times ONLY for EACH tool (not Program)

#det_time = 2, Output Rapid/Feedrate times ONLY at end for entire program

#det_time = 3, Output Rapid/Feedrate times for EACH tool AND Program

det_time : 0 # Output Rapid/Feedrate times, where?

 

# The 'stock_info' switch allows selecting to output detailed Stock Information

stock_info : yes # Display Part location, stock size/location

 

show_tool_mfg : yes #Output the tool definition - 'manufacturer' data?

show_chuck_name : yes #Output the tool definition - 'chuck name' data?

 

show_tool_details : yes # Output tool details information (20000's data)?

 

~~~~~~~~~~~~~~~~~~~~~~

~~~~~~~~~~~~~~~~~~~~~~

The setup sheet tool list reports the tools used in the selected file, arranged by tool number. The detailed tool list also includes a tool symbol and parameters for each tool.

The setup sheet operations list reports similar information, but it is arranged by operation number. The operations list also adds the following information to the detailed list:

 

¨ descriptive information about the operation (taken from comments in the toolpath parameter)

 

¨ operation time estimates

 

¨ average tool change time

 

¨ rapid feedrate

 

¨ total machining time

 

The tool list displays when you choose the tool list icon from the Setup sheet Operations tab .

Note: The heading text on these lists is defined within the list report, not on the Text Fields tab of the Setup sheet dialog box.

 

 

1. From the Setup sheet dialog box, choose the tool list icon. The tool list for the currently selected file displays in the format last selected (either detailed or summary).

 

2. To switch between tool list and operations list, choose the list content button .

 

3. To switch between detailed and summary formats, choose the format button .

 

4. To change the content of the report heading, choose Document and Title text. The Title text dialog box opens. Enter heading text and choose OK.

 

5. Choose Document, Justification to switch between unjustified and justified text (text arranged in columns).

 

6. Choose Document, Scaled To Fit to switch between a report that may exceed the page boundaries and a reduced scale image where the longest line fits.

 

7. To change the report font, choose Fonts, List fonts. Select a font and press [Esc] to close the font list and return to the tool list.

 

8. To change the report font, size, or effects (bold or underlined), choose Fonts, Choose Font. Make your selections and choose OK.

 

9. To choose margins, page orientation and other page setup parameters, choose File, Page Setup. Make your selections. To change the output device, choose Printer, select a device, and choose OK. The Page Setup dialog box reopens. Choose OK to return to the report.

 

10. Choose File, Print preview to display an image of the printed report.

 

11. Choose File, Save to save the tool list in ASCII (*.DOC) format.

 

12. Choose File, Print to print the list.

 

13. Choose File, Exit to return to the Setup sheet dialog box.

~~~~~~~~~~~~~~~~

~~~~~~~~~~~~~~~~

The Filter settings dialog box lets you set parameters for toolpath optimization, which include:

 

¨ tolerance for replacing multiple linear tool moves with a single move.

 

¨ number of points Mastercam looks ahead when filtering a toolpath.

 

¨ one-way filtering to filter a toolpath in one direction, usually for a finish toolpath, to avoid small polygonal patterns on the finish that can happen with zigzag filtering.

 

¨ optional replacement of linear moves with arcs. The Create arc options limit which planes arcs can be created in.

 

For Mill operations, Filter may create arcs in the plane you choose: XY, XZ, or YZ planes. Choose an option appropriate for your post processor configuration to handle arcs (usually designated as G17, G18, and G19 in the NC code).

 

¨ minimum and maximum arc radius.

 

For a definition of each option, click on ? in the upper-right corner of the dialog box then on the option.

Note: Default filter parameters are set on the NC Settings tab of the System Configuration dialog box, which you can reach by choosing Main Menu, Screen, Configure.

You can filter most toolpaths as they are being created. You can also filter toolpaths after generation through the Operations Manager, or filter any NCI file from the NC utils/Filter menu option. We recommend that you filter toolpaths while they are being created to maintain associativity.

 

~~~~~~~~~~~~~~~~~

HTH

ETHH

[Yogesh K. Raman]

Thanks for the reply. I'll try once I have the chance.