


                                  - 1 -



       COMMAND

       rrrroooouuuugggghhhhccccuuuutttt ---- eeeexxxxcccceeeessssssss ssssttttoooocccckkkk rrrreeeemmmmoooovvvvaaaallll mmmmaaaacccchhhhiiiinnnniiiinnnngggg

       USAGE

       rrrroooouuuugggghhhhccccuuuutttt [----ccccddddbbbbllllmmmmhhhhffffssssqqqqiiiipppprrrrnnnnvvvvooookkkk2222] [_a_r_g_s] _t_o_o_l_d_i_a [_s_t_o_c_k_r_a_d]

       DESCRIPTION

       The options following the dash are summarized here:

       ----cccc    Climb cutting mode.

       ----dddd    Dig (conventional) cutting mode.

       ----bbbb    Bidirectional cutting mode, default.

       ----llll    Light cut mode (depth = 1 x tooldia).

       ----mmmm    Medium cut mode (depth = 2 x tooldia).

       ----hhhh    Heavy cut mode (depth = 5 x tooldia).

       ----ffff    Full cut mode, default (depth = 10 x tooldia).

       ----ssss    Slow cut mode (reduced feedrate).

       ----qqqq    Quick cut mode, default (normal feedrate).

       ----iiii    Mirror image cut mode (mirror x axis).

       ----pppp    High precision cutting mode.

       ----rrrr    Rectangular (cartesian) cut mode.

       ----nnnn    No cut mode (display cutting stats only).

       ----vvvv    Void skipping cut mode.

       ----oooo    Overlap traverses by 1/2 tooldia.

       ----kkkk    Reverse longitudinal feed cutting mode.

       ----2222    Two spindle cutting mode.

       The _a_r_g_s meta-word above may have one or more of the
       following values:

       ----dddd_d_e_p_t_h     Depth of cut per pass in microns.  (relative to
                   max radius or [stock radius])











                                  - 2 -



       ----tttt_t_r_v_s      Starting traverse.

       ----pppp_p_a_s_s      Starting pass.

       ----kkkk_p_i_t_c_h     Pitch or modulus of rrrroooouuuugggghhhhccccuuuutttt traverses, cut
                   every n'th traverse commencing with traverse 0,
                   where n is pitch.

       The remaining arguments are as follows:

       _t_o_o_l_d_i_a     Actual tool face diameter in microns, mandatory.

       _s_t_o_c_k_r_a_d    Approximate maximum stock radius in microns,
                   optional.

       The default cutting regime is bidirectional at full depth
       (10 times the toolface diameter) and at normal (quick)
       feedrate.  No x-axis mirroring occurs, tool commands
       involving radial spindle motion are expressed to normal
       precision, cylindrical coordinates are in effect and voids
       are fatal (no void skipping).  Successive traverses are not
       overlapped, longitudinal feed is clockwise as viewed along
       the positive sense of the cylindrical axis, i.e., positive x
       axis and single spindle operation is assumed.  Cutting
       begins at full depth on traverse 0 and pass 0 and all
       traverses are cut in succession.

       Specification of the tool diameter, in microns, is
       mandatory.

       If portions of the stock significantly exceed the maximum
       diameter of image features, particularly when working with
       hard-to-machine materials, it will be useful to specify the
       optional stock radius.  This causes the the program's
       determination of pass depths to be based on stock radius
       rather than on the maximum radius feature of the object
       being machined.

       Roughcut and finecut are the two commands which control the
       machining of Cyberware digitized images under computer
       direct numerical control.  Although the two commands have
       many similarities and control somewhat similar machining
       processes, they have marked differences as well.  Both
       commands have relatively complex argument structures a
       thorough understanding of which is essential for ensuring
       desirable machining results. Some options may not be
       supported on a particular machining facility.

       Both commands require a valid image consisting of non-
       negative radius values the current range of which does not
       exceed available spindle travel.  Voids are normally filled











                                  - 3 -



       prior to machining but the void skipping option may be
       employed with caution.  If a restricted range of latitudes
       and/or longitudes is to be machined, it will normally be
       necessary to fill the entire image prior to setting
       latitude/longitude ranges prior to invoking the rrrroooouuuugggghhhhccccuuuutttt
       command.  This is due to the "side looking" provisions of
       the rrrroooouuuugggghhhhccccuuuutttt tool path calculational regime which requires
       some searching beyond the current range window.
       Alternatively, these exterior voids may be replaced with an
       appropriate constant value with the extset command.

       The rrrroooouuuugggghhhhccccuuuutttt command is by far the more complex of the two
       machining commands since it must accommodate and provide for
       a much wider range of circumstances encountered during the
       process of reducing rough milling stock to a reasonable
       approximation of the desired final surface. The finecut
       program must achieve a more precise result but it is able to
       do so within a much narrower range of peripheral
       contingencies and stock reduction rate limitations.

       The rrrroooouuuugggghhhhccccuuuutttt command structure is easier to understand and
       utilize when its structure is studied one option group at a
       time.  The seemingly formidable string of switch arguments
       shown in the first set of square brackets designate optional
       modes of proceeding through the stock reduction machining
       process.  This list becomes rather transparent when one
       recognizes that 9 of these letter arguments fall naturally
       into 3 modal subgroups involving direction of tool advance
       into the material, depth of cut and speed of the tool
       relative to the stock.

       ----ccccddddbbbb  These options refer to the motion of the workpiece
             relative to the cutting surfaces of the tool.  During
             full diameter slotting cuts, fully one half of the
             cutting surfaces are in contact with uncut portions of
             the approaching workpiece.  As a particular portion of
             the cutter rotates through the semicircle wherein the
             tools leading edge is in contact with the workpiece it
             first cuts in opposition to the advance of the
             workpiece then across the advance and finally
             symapathetic with the workpiece advance.  For such
             full diameter cuts both the dig (opposition or
             splitting) mode and the climb (assistance or hacking)
             mode of tool/workpiece interaction take place.

             During the machining of digitized images, either in
             cylindrical or in rectangular coordinates, once the
             initial slotting cut is completed there will be a
             strong tendency for characteristics of one or the
             other of the tool/workpiece interactions to dominate
             during subsequent rrrroooouuuugggghhhhccccuuuutttt traverses depending upon











                                  - 4 -



             the direction of the traverse.  As the succession of
             traverses advances laterally on a given rrrroooouuuugggghhhhccccuuuutttt pass
             the uncut portions of the workpiece will tend to be
             either pulled toward the tool's path (dig cutting) or
             pushed away from the tool's path.  The effectiveness
             of a given tool in forming and clearing optimal chips
             in certain materials may be heavily influenced by the
             predominance of one or the other of these quite-
             different tool/workpiece behaviors.  Furthermore, the
             quality of the cut surface may be quite different due
             to one mode or the other tending to induce undesirable
             effects such as chattering or perhaps tearing and
             splitting.

             For many materials of interest, structural foam and
             some waxes for example, the differences in cutter
             performance are sufficiently masked by relative lack
             of cutter resistance that bidirectional cutting can be
             used without jeopardizing results.  On the other hand,
             many materials, e.g., various hardwoods, metals,
             brittle plastics, etc. exhibit behavior which strongly
             recommend the preferential use of one mode or the
             other.

       ----llllmmmmhhhhffff These options refer to depth of cut in multiples of
             current tool diameter.  The light option restricts the
             depths of successive passes to one tool diameter, the
             medium option restricts these depths to two tool
             diameters, the heavy option signals your desire to
             proceed at a depth rate of five tool diameters per
             pass and the full (default) option allows pass depths
             of ten tool diameters.

             A recent addition to the rrrroooouuuugggghhhhccccuuuutttt command structure
             allows direct specification of an integer value for
             allowable pass depths.  This latter option will be
             discussed more fully as a separate topic in what
             follows.

       ----ssssqqqq   These options modify speed of cut, i.e., quick for
             nominal (default) feedrate and slow for a considerably
             reduced feedrate. The machine's feedrate override
             control is normally used for fine feedrate
             adjustments.

       ----iiii    This option modifies positive x axis orientation,
             i.e., i = mirror or reverse the sign of x axis
             coordinates.

       ----pppp    This option forces tool radius values to be output to
             the milling machine to one additional significant











                                  - 5 -



             digit where high precision is desired.  This option is
             particularly helpful in preserving radial resolution
             of essential features at severely reduced scale.

       ----rrrr    This option modifies the coordinate system, i.e., r =
             rectilinear or cartesian coordinates versus the
             default cylindrical coordinates.

       ----nnnn    This option produces a summary display of the
             machining parameters pertinent to the current state of
             the resident image without transmitting the normal
             sequence of actual "G code" instructions to the
             controller for the machining device.  This display
             enables you to review the various parameters for
             possible oversights and also provides a convenient
             compilation of machine setup parameters such as the
             actual ranges along the machine axes which will be
             involved in machining the current image.

             Frequent use of this option is strongly encouraged as
             a "filter" to verify the consistency of rrrroooouuuugggghhhhccccuuuutttt
             commands with the current state of the image and with
             the current working coordinate setup on the mill.
             Unfilled images, excessive radius ranges and other
             inconsistencies are readily identified with this
             option.  A very helpful feature of this option is the
             ability to determine the number of traverses and
             passes that will be required for a given tool diameter
             to complete the rrrroooouuuugggghhhhccccuuuutttt.  In connection with that
             information, it is useful in correlating the rrrroooouuuugggghhhhccccuuuutttt
             traverse associated with the longitudes of data in the
             neighborhood of certain features of the image, for
             example, the point at which the power went out while
             you were away and at which you'd like to resume the
             cut.

       ----vvvv    This option causes voids to be skipped thus allowing
             the machining of images which have not been filled.
             Interior voids are "bridged" by linear tool path
             vectors joining the valid data points on either side
             of the void point (interval).  Exterior voids are
             "bridged" by tool path vectors projecting to the
             latitude range boundary at constant radius.

             CAUTION --- Some releases incorporating this feature
             may not be usable in your applications due to the fact
             that exterior void skipping was implemented in a
             manner such that the tool path projection from the
             terminal non-void data points to the latitude range
             boundary was at zero radius.  In recent releases, the
             radius of the terminal non-void data point is used for











                                  - 6 -



             the radius of the projected tool path vector.

       ----oooo    This option causes the rrrroooouuuugggghhhhccccuuuutttt traverses to be
             overlapped by one half the tool face diameter thus
             providing means, in addition to depth-of-cut options,
             of controlling tool burden during rrrroooouuuugggghhhhccccuuuutttt machining.

       ----kkkk    This option enables reversal of the normal direction
             of longitudinal feed on one "special" milling
             facility.

       ----2222    This option enables two-spindle milling operations on
             the above facility.

       Multiple switches from the cutting mode group of options may
       be selected and entered on the command line immediately
       following the leading dash (-).  Each letter option entered
       must be joined with its predecessor the last of which must
       be followed by a blank space.

       The second optional argument category for this command
       designates the intended beginning longitudinal traverse
       number if other than zero.

       The third optional argument category designates the intended
       initial radial pass number, i.e., the particular annulus of
       allowed cut depths, if other than pass zero.

       The fourth optional argument category enables the skipping
       of an integral number of traverses between successive
       traverses as might be desirable on cylindrical rrrroooouuuugggghhhhccccuuuuttttssss on
       relatively low radius images where tool paths would normally
       result in considerable overlap.  The argument for this
       command is the pitch of successive traverses, e.g. 2, rather
       than the number skipped (1) to achieve that pitch.

       The integer tool diameter argument indicated in the rrrroooouuuugggghhhhccccuuuutttt
       usage message is the only mandatory argument and it
       specifies the face diameter, in microns, of the milling
       cutter to be employed for the operation.  Its specification
       is essential to the calculations necessary in determining
       the parameters controlling the angular separation of
       successive traverses.  Furthermore, tool diameter and the
       material being machined largely dictate allowable depths of
       cut and consequently the number of passes required to
       complete multiple pass rrrroooouuuugggghhhhccccuuuuttttssss.

       More importantly, however, the tool face diameter dictates
       the minimum radial level to which the cutter face may
       penetrate along a given traverse and just clear the highest
       features of the image surface lying within the cylindrical











                                  - 7 -



       sector spanned tangentially by the tool face at that minimum
       level.

       By default, the initial bed travel, rotary table and spindle
       positioning moves assume bidirectional cutting mode
       commencing with the first latitude interval (0) on the first
       longitude traverse (0) for the first (outermost annulus)
       stock reduction milling pass.  Accordingly, the horizontal
       bed is positioned at the current X0.Y0. position, the rotary
       table remains at its initial or indexed position (0) and the
       spindle positions the cutter face to a level just clearing
       the maximum feature radius or, if in effect, just clearing
       the optional stock radius.

       In view of the foregoing discussion, about the only
       restrictions regarding the use of optional switch arguments
       are that each category, if chosen, be separated by a space,
       that each category be immediately preceded by a dash(-),
       that selections from the cutting mode group be joined
       together and that, if chosen, the -d, -t, -p and -k
       designators are joined to their numerical arguments.

       The mandatory tool diameter argument must follow optional
       switch arguments and be separated from them by a space.  The
       optional stock radius argument, if used, must follow the
       mandatory tool diameter argument and be separated from it by
       a blank space.

       EXAMPLES

       The following examples of typical rrrroooouuuugggghhhhccccuuuutttt commands are
       provided to illustrate the wide range of machining
       considerations which may be addressed by judicious
       application of the various command options.

       The simplest and most often used form of the rrrroooouuuugggghhhhccccuuuutttt
       command illustrated by the command

       rrrroooouuuu 11112222777700000000

       which might be used to rough out an image, in structural
       foam for example, for which the radius range of image
       features is well within the constraints of both the
       available spindle travel as well as the effective cutter
       length.  The range of latitudes to be cut as well as the
       range of longitudes to be cut, if other than their
       respective maximums, need to be set prior to entering the
       rrrroooouuuugggghhhhccccuuuutttt command.  If it is desirable to restrict the
       minimum or the maximum radius for some reason, the
       appropriate radius range should be set in advance.  There
       are no provisions for altering the machining parameters "on











                                  - 8 -



       the fly" other than those normally available to the machine
       operator, e.g., perhaps spindle speed and feed rate
       override.

       A somewhat more involved example illustrates the next most
       common rrrroooouuuugggghhhhccccuuuutttt command usage scenario involving restarts
       following an interruption of the machining operation for
       whatever reason.  One would like to proceed directly to the
       point at which the interruption occurred and resume the
       process there rather than retrace the work already done.

       Fortunately, the rrrroooouuuugggghhhhccccuuuutttt command structure allows you to do
       exactly that upon entering the appropriate command.  The
       appropriate form of such a command would typically be
       something like

       rrrroooouuuu ----tttt22227777 ----pppp1111 6666333377775555

       and, assuming everything has been restored to the initial
       conditions, the system will seek directly the configuration
       that will result in resumption of machining along traverse
       27 to the depth allowed for pass 1 as if no interruption had
       occurred.

       Going on to an example of intermediate complexity, let's
       assume we're to machine the mirror image (x-axis) of a
       subject of relatively large size in a material offering
       considerable tool resistance, e.g., PVC.  Assume the
       available stock is 15 millimeters oversize in radius, our
       effective tool length is is only one half the radius range
       of image features and that we hope to obtain reasonable
       stock reduction rates by moderate depths of cut, using the
       traverse overlap mode to alleviate side loading and by
       utilizing dig (conventional) cuts only to enhance chip
       removal.  We might consider trying the command

       rrrroooouuuugggghhhh ----ddddiiiioooo ----dddd33330000000000000000 9999555500000000 111155550000000000000000

       at 120 millimeters, the second at 90, etc.  Let's assume
       that we observe that our milling cutter isn't handling the
       load too well or, better yet, that it overheats the
       material, gums up the flutes and the tool breaks half way
       through our second pass.  Now suppose we decide to try a 1/2
       inch roughing end mill and that we think it can handle a
       somewhat deeper overlapped cut. Since we've cleared the
       higher radius features of excess stock, we no longer need to
       specify the stock radius.  The command

       rrrroooouuuu ----ddddiiiioooo ----dddd44445555000000000000 ----tttt44445555 ----pppp1111 11112222777700000000 might hopefully get the job
       done.












                                  - 9 -



       As a final, perhaps extreme example, let's cut a final rough
       pass for the mirror image of an injection mold that we've
       just roughed out in aluminum.  We intend to follow up this
       final rough pass with a precision finecut using a fairly
       fine tool.  We want to get as close as possible to the
       finish surface as possible so as to minimize the finecut
       tool burden.  We select a 1 mm diameter tool and elect to
       invoke the dig, slow, mirror, precision, rectangular and
       overlapped cutting mode options.

       Since we are interested in going directly to the depth of
       the final rough pass, we must determine the total number of
       passes required by a 1mm tool or, alternatively, we can
       specify a depth of cut at least equal to the radius range
       for the image.  The latter essentially overrides the 10
       diameter default full depth of cut.

       Therefore, either the command

       rrrroooouuuugggg ----ddddssssiiiipppprrrroooo ----pppp4444 1111000000000000

       or the command

       rrrroooouuuu ----ddddssssiiiipppprrrroooo ----dddd55550000888800000000 1111000000000000

       should, with some luck and a fair amount of time, accomplish
       the task.
































