PC Electronic Plus/PC Electronics Plus (Most Significant Bits)(1995).ISO/me/me.doc

Text File | 1994-11-27 | 30KB | 800 lines

                                                        November 24, 1994


                          INTRODUCTION


ME is a program designed to help manufacturing engineers,
estimators, CNC programmers, inspectors, machinists, and other
technical personnel in the metalworking industry.  I have worked in
these fields for the past eighteen years, and a significant portion of
my working time has been spent searching through reference books
for data and making manual calculations based on those data.  After
reinventing the wheel countless times in this fashion, I decided to
make my life easier by creating a program which would give me
instant access to much of the information I needed for my work.  I
have used ME on a daily basis for the past six months - it performs
as intended and helps me in many ways.  I have decided to share
this program with the manufacturing community and perhaps
expand it significantly if the feedback is encouraging.

ME is a DOS program which will run on virtually any MS-DOS
computer in existence.  It will run, with acceptable speed, on a
384K 8088 with monochrome monitor and one floppy drive.  I like
to run it as a windowed DOS application in Windows, where I can
access it from inside other programs.  I find that 285K of memory
are enough in the .PIF file.  ME is a plain program, menu-driven
and friendly, but the emphasis is on function and not glamour.  It
requires a very short learning curve, and will be useful to
metalworking personnel of all experience levels.




                          OVERVIEW OF FEATURES


THREADS

complete dimensional data for nearly two hundred of the most
commonly used threads, including UNC, UNF, UNEF, UNJ, NPT,
ACME, and ISO

standard and close-fit thread classes

wire sizes and dimensions for measurement

suggested tap drill and tap class

root radius limits (UNJ)

minor diameters required for various percentages of thread
engagement

inch or metric display



MATERIAL WEIGHTS

twenty one different materials

shapes include hexagonal, octagonal, rectangular, square, round,
and tubular

inch or metric dimensional input

output in pounds and kilograms



MATERIAL HARDNESS

Rc, Brinell, and PSI comparisons



DRILL DEPTHS

center drills #00 - #8 to achieve a chamfer of desired diameter

countersinks of 82, 90, and 120 degree included angles to achieve a
chamfer of desired diameter

spot drills of 90 and 130 degrees,  to achieve a chamfer of desired
diameter

twist drills of 118 and 135 degree included angles to achieve a
full-diameter hole of desired depth (including compensation for
width of chisel point)



FEEDS AND SPEEDS

milling and turning operations

twenty different material categories

nine types of cutting tools

output includes machining time and horsepower requirements

output in interactive format - any output value can be modified with
immediate update of all  dependent outputs

input and output can be independently toggled between inch and
metric



CIRCULAR FEEDRATES

feedrate compensation for circular milling




                             OPERATION TIPS


the menus are case sensitive

if you press a key and nothing happens, you are probably pressing a
key that's not on the current menu or are inputting an illegal value

at a screen used for inputting information, the Esc key will take you
back to the previous screen at any time

at any output screen the 'z' key will take you directly to the main
menu

the current input and output modes are displayed in the upper right
corner

input cannot be a calculation - input "5", not "3 + 2"

inch and metric input cannot occur at the same screen.




                                  Main Menu


At the main menu, the six major options mentioned previously are
available.  Additionally, there is an option to shell out to DOS (y)
and an option to toggle between inch and metric input mode.  The
current mode is indicated in the upper right corner of the screen.
The input mode is modal, and will stay in effect until changed by
the user.



                             (c)  circular feedrates

When an end mill is cutting a straight line, the contact point of the
cutter is moving the same distance as the centerline of the cutter.
When the same tool is externally profiling a radius, the centerline is
moving further than the contact point - when internally profiling, the
centerline is moving the smaller distance.  As the centerline always
moves at the programmed feedrate, that feedrate must be adjusted
when machining a radius if the contact point of the cutter is to move
at the desired rate.
The menu provides the four possible combinations of inputs needed
to calculate this adjustment.  Options 'a' and 'b' provide for external
interpolation, options 'c' and 'd' for internal.  Options 'a' and 'c' are
used when the blueprint identifies the arc with a radius size - this is
normal when the arc is part of a continuous profile.  Options 'b' and
'd' are used when the blueprint specifies a diameter size - more
common when the circle covers 360 degrees.

There is no option to toggle inch/metric input mode here because it
is not needed.  As long as all input values are in the same mode, the
output will be correct.

Feedrate Adjustment Menus

The first value to be input is the radius or diameter to be machined.
This value will come from the blueprint.
The tool diameter is input next.  The program checks for negative
values and tool radius larger than part radius in the case of internal
interpolation.  If your input is rejected, check for these possibilities,
and be sure that you are not trying to mix inch and metric input.
The program next prompts for linear feedrate - this is the rate you
would feed the tool in a straight line (the uncompensated feedrate).
Input in distance per revolution or distance per minute.

The adjusted feedrate will be output along with a summary of the
inputs.

If you want to do another calculation, enter 'y'.  Any other key will
return you to the main menu.



                           (d)  drill depths

A calculation that CNC programmers and machinists make
repeatedly is how deep to send a particular type of drill or
countersink to achieve the desired result.


Center Drills

Options 'a' thru 'j' involve standard center drills (also known as
combination drill and countersinks).  The problem is how deep to
drill to produce a chamfer of a given diameter at the face of the
workpiece.  The user must select a center drill of a size capable of
achieving this diameter - after the tool is selected, the program
displays the high and low limits for the tool, and rejects inputs
outside those limits.  If you select a tool and find that it won't
meet your needs, use the Esc key to go back one screen and get a
different one.  The only input required is the desired chamfer
diameter.  Output will be a summary of the inputs and the calculated
depth in both inch and metric units.


Countersinks

Options 'k' thru 'm' involve standard countersinks.  The problem is
how deep to send a tool of a given included angle, with a flat of
known diameter on the end, to produce a chamfer of a given
diameter at the face of the workpiece.  The user selects a
countersink with the included angle specified on the
blueprint.  The input screen first asks for the required chamfer
diameter.
The diameter at the small end of the tool is next requested.  As a
reminder, the maximum value allowed is displayed, which must be
smaller than the chamfer diameter.  Output will be a summary of the
inputs and the calculated depth in both inch and metric units.


Spot Drills

Options 'n' thru 'o' involve standard spot drills.  The problem is
familiar - how deep to drill to chamfer the correct diameter.  Input is
the chamfer diameter required and the drill diameter, which in this
case must be larger than the chamfer diameter.  The program, taking
into account that spot drills have a chisel point on the end, of a
width proportionate to their diameter, outputs the required depth.


Twist Drills

Options 'p' and 'q' involve twist drills.  Blueprints normally specify a
drilled hole of a specific depth - but this means the full diameter of
the drill must go to that depth, rather than the point of the drill.
Input is the full-diameter depth required and the drill diameter.
CNC programmers and machinists commonly use multipliers of .3
and .207 times diameter to compensate for the length of 118 and
135 degree drill points, respectively, but these figures assume a
sharp point on the end of the drill.  The program, taking into
account that twist drills have a chisel point on the end, of a width
proportionate to their diameter, outputs a more accurate calculation.




                         (f)  feeds and speeds

An important part of the work of many manufacturing planners,
estimators, and CNC programmers in the metalworking industry is
the advance calculation of machining times for specific
combinations of workpiece materials, cutting tools, and machine
tools. Such people need a consistent and logical  method for
calculating efficient feedrates and spindle speeds - not too
slow, which is wasteful of machine time and manpower, and not too
fast, which is wasteful of tools and can increase costs in the long
run.  While optimal cutting parameters cannot always be calculated
ahead because of the wide range of subjective variables (variations
in material, machine rigidity, workpiece rigidity, clamping integrity,
etc), it is possible to establish reasonable starting points which can
then be optimized as necessary after visual observation of the cutting
operation at the machine.  That is the intent of this section of the
ME program.

The initial screen displays twenty material categories and, in
parentheses, a specific material designation which is representative
of that category.  Some programs exist which try to give specific
data for hundreds of different but similar materials - I have not
found this degree of detail to be especially helpful in my own work.
Remember, the purpose of this program is to provide starting points -
a knowledgeable and observant person at the machine will
always be the best judge of what is optimal.

After selection of a material category, the user is presented with a
selection of cutting tool types.

hss twist drill

An input screen appears which displays the currently chosen
material and tool type and asks for a tool diameter.  The maximum
and minimum diameters allowed by ME are also displayed, in
inches or millimeters depending on the active input mode.
The next prompt is for the hole depth - this is needed to determine
machining time and also to see if another prompt must be issued.  If
the ratio of hole depth to drill diameter is greater than or equal to
3:1, it is common practice to reduce feedrates and spindle speeds.
The larger the ratio, the greater the reduction.  This reduction is
probably more valuable with manual machines where regular drill
retraction or pecking is not easily done.  With CNC machines,
unless the ratio is quite large, it is probably less important.  In any
event, the user has a choice as to whether or not to apply the
compensation.

The output screen is now displayed.  This screen displays complete
information for the machining process selected, and a menu at the
bottom which allows the user to make changes to the data which
result in immediate updates to all data which are logically affected.
As this output screen is similar no matter which material or tool has
been selected, I will give a detailed explanation once and only
discuss the differences for specific tools as they occur.

Note that the upper right corner now displays status for input mode
and output mode.  The user can toggle the entire display between
inch and metric with the 'x' menu option.  Changing the input mode
(option 'X') will be discussed later.


The MATERIAL, HOLE DEPTH, TOOL, and tool DIAMETER
are based on user inputs.


DEPTH/DIAMETER is the ratio of hole depth to drill diameter.


HARDNESS displays the approximate Brinell and Rockwell "C"
material hardness values upon which the machining data are based.
These numbers will always reflect the low end of possible values for
the chosen material.  If the material you are machining has higher
values, spindle speeds, and sometimes feedrates, must be reduced.
A very general note is included at the top of the display screen as a
reminder to this effect.  The actual reduction necessary for
productive machining may vary from the values in the reminder.


MINUTES displays the machining time for one hole and the time
for all holes. The initial display will assume that one hole is being
machined, so both times will be the same.  The value for the total
number of holes can be modified from the menu, as will be discussed later.


SFM displays the surface feet per minute calculated for the
material/tool combination.
SMM displays the surface meters per minute calculated for the
material/tool combination.


RPM displays the spindle speed calculated for the material/tool
combination.  This will not change when the output units are toggled.


IPR displayes the feedrate in inches per revolution calculated for the
material/tool combination.
MPR displayes the feedrate in millimeters per revolution calculated
for the material/tool combination.


IPM displayes the feedrate in inches per minute calculated for the
material/tool combination.
MPM displayes the feedrate in millimeters per minute calculated for
the material/tool combination.


HP displays the power required at the motor (horsepower)
KW displays the power required at the motor (kilowatts)


MMR(ci) displays the material removal rate (cubic inches per
minute)
MMR(cc) displays the material removal rate (cubic centimeters per
minute)



                       Menu Options (case sensitive)

(t) Tool diameter - the 't' key will bring up an input box which can
be used to modify the current tool diameter.  The minimum and
maximum allowable values will be displayed.  The Esc key will back
out of the box with no changes being made.  After the new diameter
is input, all values on the display which depend on the tool diameter
will be automatically updated.
The 'Shift' key combined with the 't' key will increment the tool
diameter by approximately one percent.

The 'Ctrl' key combined with the 't' key will decrement the tool
diameter by approximately one percent.

The ability to use these 'Shift' and 'Ctrl' key combinations allows the
user to play some fast "what-if" or goal-finding games.  For
example, if you only have a five horsepower machine and the tool
you initially chose requires seven horsepower, 'Ctrl  t' will quickly let
you find the largest tool possible for that machine.  As the tool
diameter decreases, the power requirement and some other values
change right along with it.  These key combinations are available for
all menu options up to and including "Spindle override".


(l)  hole depth - the input box will allow modification of the hole
depth


(h)  number of holes - the input box will allow modification of the
number of holes


(d)  option unavailable  -  these options do not apply to the current
tool type
(w)  option unavailable                        "
(i)  option unavailable                        "


(f) Feed override - the input box will allow modification of the feed
override, expressed as a percentage of the feedrate initially
calculated by the program

(s)  Spindle override - the input box will allow modification of the
spindle override, expressed as a percentage of the speed originally
calculated by the program


(r)  Rpm limit - the input box will allow the user to set the maximum
spindle speed of which a particular machine tool is capable.  The
limit is initially set at 200,000 RPM, which is intended to mean "no
limit".  If the program calculates a spindle speed for a tool which
exceeds this rpm limit, the RPM display will show the value for the
rpm limit, but an asterisk will appear beside it to indicate that it has
been restricted, and underneath it, in parentheses, will be a number
showing what percentage this restricted value is of the calculated
value.  The rpm limit is modal.


(e) spindle efficiency - the input box will allow modification of the
spindle efficiency.  This figure, expressed as a percentage, allows
the planner to fine tune the power requirement value for a
machining operation.  This is because some machines are more
efficient at delivering power to the spindle than others - thus some
machines must have a higher power rating than others to do the
same job.


(x)  set metric output - toggles the display between inch and metric
units


(X)  set metric input - toggles the input mode between inch and
metric.  The user can display in one mode and input in the other.


(y)  previous menu - return to the previous menu - all displayed
values are initialized with the exception of the rpm limit, which is
modal


(z) main menu - return to the main menu - all displayed values are
initialized with the exception of the rpm limit, which is modal



indexable drill

An input screen appears which displays the currently chosen
material and tool type and asks for a tool diameter.  The maximum
and minimum diameters allowed by ME are also displayed, in
inches or millimeters depending on the active input mode.
The user is next prompted for a hole depth - this is needed to
determine machining time.
The output screen is now displayed. It is identical in content and
operation to the display for twist drills.



hss spade drill

Input and output screens are identical to those for indexable drills.



gun drill

Input and output screens are identical to those for indexable drills.



hss end mill

An input screen appears which displays the currently chosen
material and tool type and asks for a tool diameter.  The maximum
and minimum diameters allowed by ME are also displayed, in
inches or millimeters depending on the active input mode.
The user is next prompted for the number of flutes, or cutting
edges, on the tool.  An arbitrary upper limit of twelve is built into
the program.
The next value requested is the width of cut.  This cannot exceed
the tool diameter.
The fourth prompt is for the depth of cut (distance along the spindle
axis). The generally accepted upper limit, beyond which results
become less predictable (and less productive), is one and one half
times the tool diameter. This limit has been built into the program.
The output screen is now displayed.  Differences from the features
previously discussed are:


DEPTH OF CUT - note that this value cannot exceed one and one
half times the tool diameter - if the tool diameter is reduced, the
program checks the depth and reduces it also, if necessary.


WIDTH OF CUT - note that this value cannot exceed the tool
diameter - if the tool diameter is reduced, the program checks the
width and reduces it also, if necessary


IPT displays the feedrate in inches per tooth (flute) calculated for
the material/tool combination.
MPT displays the feedrate in millimeters per tooth (flute) calculated
for the material/tool combination.


(l)  Length of pass - the input box will allow modification of the
pass length

(p)  number of passes - the input box will allow modification of the
number of passes


(d)  Depth of cut - the input box will allow modification of the
depth of cut - this cannot exceed one and one half times the current
tool diameter


(w)  Width of cut  - the input box will allow modification of the
width of cut - this cannot exceed the current tool diameter


(n) Number of flutes - the input box will allow modification of the
number of cutting edges



                                  WARNING

The user bears responsibility for correct tool selection.  For
example, most experienced persons would prefer a two flute end
mill over a four flute for heavy roughing cuts in aluminum, owing to
its greater chip clearance and freer cutting action.  The opposite
might be true when machining steel.  The program will, in both
cases,  show twice the feedrate for a four flute tool.  This might
sound good to the unwary, but results at the machine would not be
what was expected.  The ME program is an excellent planning aid,
but is not a substitute for experience.



carbide end mill

Inputs and outputs are identical to those for hss end mills.



face mill

An input screen appears which displays the currently chosen
material and tool type and asks for a tool diameter.  The maximum
and minimum diameters allowed by ME are also displayed, in
inches or millimeters depending on the active input mode.
The second prompt is for the number of inserts, or cutting edges, on
the tool. An arbitrary upper limit of one hundred is built into the
program.
The next value requested is the width of cut.  This cannot exceed
the tool diameter.
The last value requested is the depth of cut (distance along the
spindle axis).
The program does not try to take into account the many sizes and
geometric orientations of the inserts in face mills.  The maximum
depth of cut recommended for a specific face mill is a direct
reflection of these factors.  A limit on depth of cut has not been
built into the program.  The user is responsible for inputting realistic
depth of cut values.

The output screen is now displayed.  It is identical to that for end
mills, with the exception that option (i) Number of inserts replaces
option (n) Number of flutes.



hss reamer

Input and output screens are identical to those for indexable drills,
with the exception that power requirements and material removal
rate are not displayed.  The amount of material removed by the
reamer is not always known.  In any event, reamers are typically
used to remove very small amounts of material, and these figures
would have no practical value.



turning

An input screen appears which displays the currently chosen
material and tool type and asks for a turn diameter.  Note that this
must be the diameter actually being machined, rather than the
diameter of the material.
The next value requested is the depth of cut per side.  The value for
depth of cut cannot exceed one inch.   This limit will not prevent
some pretty unlikely combinations from being accepted.  Therefore,
the user is responsible for inputting realistic depth of cut values.

The output screen is now displayed.  It is identical to that for end
mills, with the exception that option (t) Turn diameter replaces
option (t) Tool diameter, and options (w) and (n) become
unavailable.

The output for turning is very generalized.  It assumes the use of
titanium- coated inserts under conditions of moderate roughing.
Feedrate can be adjusted down for finishing passes or up for heavy
roughing.  Speed can be adjusted up for finishing or down for heavy
roughing.  The user must know what he is trying to accomplish and
how to do it.  The machining times and power requirements are the
most valuable outputs here - the speeds and feeds are merely
references based on the combined recommendations of industry
professionals and my own experience.




                           (h)  hardness equivalents

There are three measures of steel hardness most commonly used in
the American metalworking industry.  They are Rockwell "C",
Brinell, and PSI.  The planner, CNC programmer, inspector, or
machinist often needs to convert a value from one scale into an
approximate equivalent on another.


Hardness Equivalence Menu (Steel)

The user selects the scale for which he has a value.


The input screen prompts for the known value.  Minimum and
maximum acceptable values are indicated.
The output screen shows three columns of eleven values each, with
the left column containing the values of the chosen scale.  The sixth
(middle) value in the left column will be the closest available to that
input by the user.  By reading from that value across the screen, the
equivalents may be obtained.

The '+' key will simultaneously scroll the tables by one value larger.
The '-' key will scroll one value smaller.  In this way, the entire table
of values may be browsed.




                             (t)   thread data

CNC programmers, machinists, and quality control personnel have
frequent need for dimensional data on threads.  This information is
in print, but complete analysis of a specific thread usually requires
that half a dozen manuals be searched and error-prone calculations
be made.  This is messy and time-consuming, and works poorly
when several persons need data from the same source
simultaneously.  The ME program displays a complete summary of
dimensional data for nearly two hundred of the most commonly
encountered threads.


Thread Menu

A menu of seven thread categories is displayed.

The next screen displays a menu of the specific threads within the
selected category.

The output screen displays data for the selected thread.  I will not
explain each output, the presumption being that a person who has
need of the data will understand what it means. The output can be
toggled between inch and metric with the 'x' key.  Entering a 'y' at
the display screen  returns to the Thread Menu.  Any other response
returns to the Main Menu.



                         (w)   material weights option

Estimators, process planners, and buyers must frequently calculate
the weight of material of a given composition and shape.  CNC
programmers, fixture designers, or machinists might need to
calculate the weight of a workpiece to make sure a machine or
fixture is capable of supporting it, or for safety considerations.  The
ME program displays a complete summary, including material type,
shape, dimensions, and weight in pounds and kilograms.


Material Weight Menu

A menu of nineteen materials is displayed.

The next screen displays a menu of supported shapes.



hexagonal
octagonal

An input screen appears which displays the currently chosen
material and shape and asks for the dimension across the flats.
The next prompt is for the material length.
Output is displayed.



rectangular

An input screen appears which displays the currently chosen
material and shape and asks for the material length .
The  next prompt is for the material width. The final prompt is for
material thickness.
Output is displayed.



square

An input screen appears which displays the currently chosen
material and shape and asks for the length of one side of the square.
The next prompt is for material thickness.
Output is displayed.



round

An input screen appears which displays the currently chosen
material and shape and asks for the material diameter.
The next prompt is for the material length.
Output is displayed.



tubing - o.d. and i.d.

An input screen appears which displays the currently chosen
material and shape and asks for the material outside diameter .
The next prompt is for the material inside diameter.
The final prompt is for the material length.
Output is displayed.



tubing - o.d. and wall

An input screen appears which displays the currently chosen
material and shape and asks for the material outside diameter.
The next prompt is for the material wall thickness, which must be
less than half the diameter.
The final  prompt is for the material length.
Output is displayed.




                             (y)  DOS Shell

This feature allows a temporary exit to DOS.  While at the DOS
prompt, type "exit" followed by the Enter key to return to ME.




                             SALES PITCH


I spent many hours on this project - gathering and interpreting the
data was a big job.  Learning C and writing the program took up
many long evenings.  I have some thoughts on ways the program
could be expanded.  In addition to more data and more types of
calculations, I can see value in such things as report generation and
menu/mouse support.  In order to improve the program, I will need
some feedback, both financial and intellectual.  If you like ME well
enough to use it on a regular basis, I think a check for twenty dollars
would be a fair deal for both of us.  If you register, you'll get the
next version free of charge.  Along with the check, send your
comments and ideas for improvement.  What do you especially like
or dislike about the program?  Does it help you do your job?  What
would you like to see new or different about it?

If you need a program like ME but don't think it's worth twenty
dollars, tell me why.



                                              Michael Rainey
                                              103 Fawn Lane
                                              Kings Mountain, NC  28086
                                              704-435-2459
                                              MRAINEY - Genie