================ Gears machining by milling tools =================== 1 That's me! 
      
      My name is Fabio Sada.
      I was born in 1954 in Milano, where i studied up to University and
      where i have been working since 1978 as production technologist at
      a primary firm active in heavy industrial plants supply (coil mills,
      continous casting etc).
      During my job I worked about machining methods, CNC part-programs,
      setup equipements, tools also regards to gear machining ( hobbing,
      rack-cutter machining and grinding) so that I ideated a new way
      of machining gears by milling instead of by hobbing, and I created
      some EDP tools for simulating new process and make ordinary
      calculations about gears, but without testing this new way in my job.
      It would be for me very satisfying if any gear manufacturer be
      interested in this idea and try to put it into real practice.
      

      -Fabio Sada
      -Via San Pancrazio 20
      -20060 Gessate (MI) - Italy
      -
      e-mail : sada.gessate@tiscalinet.it  
      


4     Introducing
      The machining of gears involute is actually carried out by by using
      hobs or rack-cutter, on their own proper machine, usually followed by grinding.
      Altough for small modeles hobbing technology for machining involute surface
      before grinding is probably the best one, for large modules hobbing
      takes a lot of problems, since both the
      machine tool and tools become very expensive and very little flexible.
      Then it is necessary to handle a very heavy and delicate tooly, while
      machine table is required to turn at high speed without any precision loss.
      Gear machining by milling may be a good answer to such problems, with
      machining time very interesting and a lot of further advantages.
      For low-quality gears milling might be used as the final involute machining.
      In the following chapters we'll show that gear milling is geometrically
      correct, technically executable and economically convenient, and that
      for large modules the hobbing technology is obsolete, although
      the only apparent technical evolution of hobs and hobbing machines.


5     New! create involute by milling
      !! This new way uses a generating method and consists of creation of
         micro-planes or micro-lines that belong to involute surface.
       This may happen because involute surface has some characters:.
         -If you imagine to cut the gear with a plane tangent to base cylinder,
         you will obtain some straight lines costanly sloped as base helix angle;
         There will be more than one parlel lines for each side, and their distance
         (in trasverse and normal directions) is equal to respectively base trasverse
         pitch and base normal pitch.
         While tangent plane rolls over base cylinder, the lines move (but remain equally
         spaced ad oriented each other) according to the very simple rolling law
         over base cylinder:

        [1]   delta X = Rb * delta ROT [radiants]

         If the cut contains the whole central teeth, as for gears with a few teeth,
         you will find that the distance between first left-side line and first right-side line
         of central teet is equal to trasverse (normal) base thickness.
         This happens also if you imagine anyway to continue involute profile forward
         base circle for any number of teeth.
         Then (and this are probably the most importan carachteristic) the
         teeth surface immediately close to section is always normal to our
         imaginary plane, and this surface is anyway always convex, so that may be
         substituted by micro-planes tangent to real surface, with a small
         positive error.
         A daily show of this simple rules comes from span measurement:
         just imagine to substitue plates with a milling tool and place it at
         the first contact.
         I defined two different machining modes, each with its own advantages:.
         CONTINOUS MODE:.
           -The gear is placed on a rotary table (B-axe).
           -The milling tool is placed on a square-head indexed as base helix angle.
           -Its edge lays constantly in Z axe on plane tangent to base cylinder.
           -The gear rotates (B) and mill moves (X) according to rolling law;
           In each moment a circular arc substitutes the real generating line.
           -Final form error depends upon milling path width, tool diameter and
           mimimum curvature radius (innest X position).
        In case you wish to have a constant feed along involute profile, it is
        necessary to fit X-Feed according to [fig26A][fig27A][fig28A] :

        [2] FeedX = Feed on profile * rb / Rcurv

        It is also necessary to verify that this value doesn't become
        too large, as curvature radius becomes very small.
       [fig24A][fig04U][fig05U][fig19U][fig20U].

         MULTI-PLANE MODE:.
           -The gear is placed on a rotary table.
           -The milling tool is placed on a square-head indexed as base helix angle.
           -Both gear and tool are moved in any position that respects rolling law.
           -In this X-B fixed positions the milling tool moves along Z and creates
            a small plane tangent to real involute surface.
           -Final form error depends upon the number of planned cuts and minimum
            curvature radius (innest X position).
           -A special case is made by first rough machining by a thin milling tool
            [fig33A][fig34U].

      Both methods may be considered as a special condition of modified rolling,
      in case tool pressure angle becomes ZERO.

5.1   Machine setup for both milling modes.
      Toolaxe index = base helix angle.
      Zero-offset X  : Centerline of rotary table.
      Zero-offset Y  : where you want, but better on an intermediate section
                       where it is possible to center a pre-existing spacewith.
      Zero-offset Z  : Centerline of rotary table.
      Zero offset B  : Centerline of tooth or spacewidth, with their
                       own delta-X contribution; If center of tooth is used,
                       for B=0 then X cut position must already be equal to half trasverse
                       base thickness.
      Tool position T along Z:

        [3]  T = rb + rtool

      Rolling law during movement:_

        [4]  delta B [rad] = delta X / rb



        [5]  B = B0 + X / rb

      Helix law for different Y-levels:

        [6]  delta B-offset [rad] = 2 * 3.14159 * Y / lead

      Feed fitting law , only in continous mode:

        [7]  Feed X = Feed on profile * (rb / X)

      Distance of eventual 2nd rear tool, that operates over a close teeth

        [8]  L = normal base pitch



6     Mode 1 : Continous rolling milling mode
      This method may be carried out ONLY after spacewidth rough machining!
      [fig02A][fig03U], better if followed by a proper root undercut made
      with rounded mill.
      [fig12A][fig13U] show innest position layout.
      [fig15A][fig16A] show start and arrive conditions.
      In this machining mode milling tool center moves along X over a plane tangent
      to base cylinder, while gear on the table turns, according to
      rolling law shown before, with a simple NC
      command from (X1,B1) to (X2,B2) with Z=base radius.
      In case the gear is not exactly centered on the table, the movement
      must involve also Z-axe and must be shared into n partial positions,
      each of them with properly re-calcoulated X-B intermediate values
      according to value and current direction of center desplacenment vector; in
      this case some form error occours since a continue formula is
      linearized into n steps.
      Extreme positions may be easily calculated according to tip diameter
      and (for example) active profile starting diameter.
      Both these values may be modified according to milling path width
      and tool angle:

         [9]  Extra radius = path width / 2 * TAN(beta0)

      In enclosed example this extra is considered only for multi-cut planning.

      Form error: both values of path width and tool diameter lead to
      a first value F1 representing the arrow operated by milling tool movement
      in local tangent plane [fig19U].

        [10]  F1 = Rtool - ( SQR ( Rtool ^ 2 - (path width / 2) ^ 2 ) )

      This value and minimum curvature radius lead to the true form error F2
      [fig20U][fig27A]:

        [11]  F2 = rcurv -( SQR ( rcurv ^ 2 - F1 ^ 2 ) )

        (tabled in [fig20U] with entrance in column 1)
        For example, for Dtool=250 mm and pathwidth=60 mm you have F1=4,50 mm.
        In case of minimum curvature radius = 75 mm you may have a form error
        = 0,122 mm , that lowers to 0,017 mm for radius=500 mm .
        Although these are good values, they may be easily reduced:
        if you operate an extra-position of tool along Z, UNDER the level
        of tangent plane and equal to 1/2 of F1 value (2,24 mm in example),
        then real error F2
        lowers very much, since the true value F1 to be considered is the
        half ([fig20U] with entrance in column 2):

        [12] F2 = rcurv -( SQR ( rcurv ^ 2 -( F1 / 2 ) ^ 2 ))

        leads to better values:


: rcurv =  75   form error 0,030 mm instead of 0,112 mm
:       = 517   form error 0,004 mm instead of 0,017 mm
        A further improvement may come from insert cutting edge, in case
        it offers a flat front edge.
        In any case form error [fig04U][fig05U] lowers when tool diameter increases
        or path width reduces [fig18A].


7     Mode 2 : Multi-plane machining with stopped table
      In this machining mode the milling tool moves along its own plane while
      other machine axes are stopped, so thet it may be carried out
      also over whole-teeth, not rough machined gears, and over machines with
      a good static precision but not a good dynamic one.
      [fig12A][fig13U] show milling in innest conditions.
      In this case I suggest to operate first both cuts on left and right flank,
      and then increase both X-position and cut depth.

      Also in this case extreme positions may be easily calculated according to tip diameter
      and (for example) active profile starting diameter.
      Both these values may be modified according to milling path width
      and tool angle:

         [9]  Extra radius = path width / 2 * TAN(beta0)

      In enclosed example this extra is considered only for multi-cut planning.
      [fig06A][fig07A][fig08A][fig09A][fig10A][fig11A].

      A proper EDP software may be used for planning cutting positions, so to
      have equal and minimum form error for each integer quantity of cuts.
      Single unit cut will be repeated for all teeth and for all axial sections planned.
      Since form error depends upon curvature radius, best results will be for
      gears with a lot of teeth , but in case of further grinding
      this is not a problem anyway.
      In case of spur gears it is better to machine the whole facewidth
      at one time for each planned position.


8     Cut with two spaced milling tools
      In case you use two equal milling tools spaced as the normal base pitch
      [fig12A][fig13U], you will machine at one time two different
      surfaces on adiacent tooth, relative to 2 different curvature radius
      according to:.

        [13]  R rear = R front + normal base pitch * COS(beta0)

      For better understand what happens with two milling tools, it is
      necessary to define Krc ratio that represents cut-lenght operated by
      rear milling tool and whole cut lenght:

        [14]  Krc =  (Lctot - normal base pitch * COS(beta0)) / Lctot

      That shows covering action of rear milling tool.

8.1   Continous mode
      In case of two milling tools in continous mode, active path of
      front tool may begin at an intermediate position, since
      rear tool has already machined initial path during cut before.
      Best condition occours when Krc value is exactly 0,50 , that means
      that both tools begin active cut at the same time other than
      along the same path lenght.
      Obviously the first cut for each axial set of cut must be done
      along a whole path.
      In this way machining time may be reduced up to 50%, expecially
      when Feed value along X must be kept constant, and the reduction
      is anyway good also when it is possible to fit feed value according
      to current curvature radius of REAR tool.
      In fact, the position difference over profile path corresponding to
      a fixed difference of curvature radius becomes smaller as curvature
      radius lowers, so that with feed auto-fitting the front tool has
      a real feed over profile lower than optimal one.
      Cut starting position of front tool along the path may be reached
      with a high feed with correct X position, or with a small tool
      desplacement along X .
      - For values of krc up to 0,50 [fig27A] the first contact is done by
      front tool, and feed fitting may be referred to front tool position;
      As rear tool begins to cut, feed must reduced since must be referred
      to rear tool position; Milling path along X is constant for any value
      of krc.
      - For values of krc over 0,50 [fig28A] the first contact is done by
      rear tool, and whole feed fitting is referred to its position.

      For example, in case of gears in example we have following machining time
      for each cut path, for a reference feed on profile = 100 mm/min
      in both fitted and not-fitted feed (values T100P and T100C in [fig25A][fig26A]):.


:                  WITH NO fit       WITH fit
: PINION:
:  with 1 tool  :     0,901           0,609
:  with 2 tool  :     0,522           0,424
:
: WHEEL:
:  with 1 tool  :     0,649           0,581
:  with 2 tool  :     0,380           0,357
      It is clear that feed fitting is more convenient in case of pinion,
      when curvature radius changes very much in relativ value, and then
      use of 2 tools is more convenient for machining wheels, since both
      front and rear cut move along the profile with small real feed
      differences.
      Best machining results occour when krc value is close to 50% and it
      is possible to fit feed value continously.
      Warning: feed fitting is not a matter of CNC performances ( since it
      is always possible to share cut path into 10-20 steps and assign a
      proper feed value to each one ) but depends upon the position error
      of B-X axes when feed changes: it shouldn't be a problem for a
      modern machine, but it could be the same.
      Instead of in order to reduce machining time, second tool might be
      placed a little more spaced and be used
      for reducing material stock to be removed by front tool along the
      external path ( usually corresponding to greatest amount of over-stock).
      In this case whole path must be run by front tool, even with a certain
      penalty since rear tool commands feed value anyway.

8.2   Multi-plane mode
      In this case the second tool allows to reduce the number of cuts, and
      each cut operates at two different curvature radius on two following teeth.
      Since tool distance is strictly defined, the cuts planning must be
      optimized in reference to front tool or rear tool extreme positions,
      so that the number of cuts for a certain form error doesn't succeed
      in reaching the half value [fig06A] [fig09A] [fig07A] [fig11A].
      Also in this case the value krc leads to refer planning mode to
      front or rear tool extreme positions.
      A simple simulation shows that the distance between two cuts ( for an
      assigned form error ) become larger as curvature radius reduces: this
      means that a cut planning referred to rear tool will be certainly
      satisfying if properly translated to front tool.
      It is only necessary to check relative position between innest rear tool
      position and outest front tool position.
      For values of krc over 0,5 it is better to plan cuts in reference
      to tip circle curvature radius ([fig10A] with plan edge=Re).
      For values of krc up to 0,5, it is better to plan cuts in reference
      to a virtual external circle corresponding to innest cuvature radius +
      2 x [base normal pitc] * COS(beta).
      in order to assure complete covering to front tool position ([fig11A]
      with plan edge=ri+2*P).
      For example, we show cut plannigs and their form error for
      gears in example:


:                  n=8   n=7   n=6   n=5   n=4   n=3   n=2
: PINION:
:       1 tool :  0,071 0,095 0,131 0,196 0,327 0,634 1,769
:       2 tools:  0,023 0,031 0,044 0,065 0,108 0,210 0,584
:
:  WHEEL:
:       1 tool :  0,016 0,021 0,030 0,045 0,074 0,146 0,403
:       2 tools:  0,005 0,006 0,008 0,012 0,020 0,039 0,108
      That shows how second tool is convenient also in multi-plane mode.


9     Something more : first rough cut with disc milling tool
      First rough cut may be done by a thin milling tool disc-shaped,
      instead by an ordinary double-cone milling tool, with lower chips
      removal and lower machine stress [fig33A][fig34U].


10     Something more : Milling by an hobbing machine
      Milling machining of gears might be carried out also by hobbing machines
      in both cutting modes, in case the machine offers the chance of positioning
      milling tool in tangential direction.
      In case stroke lenght along this axe be too short ( then not so good for
      machining large wheels with large curvature radius ) a good help might come
      by allowing to inclinate tool axe in transverse plane, for example as
      normal pressure angle, so that milling path always happens close to
      machine center-line [fig16A][fig17A][fig21A].
      In this case tool moves along X-Z axes instead of along Z axe or X axe alone.


11     Limits in machining gears by milling
      Since both machining modes shown above operate a substitution of real
      expected surface with something different ( an arc in case of continous
      mode, and a plane in multi-cut mode) some form errors occour.
      This means that gears milling may be used without problems ONLY in
      case of further grinding (expecially for multi-plane machining mode)
      or in case of low-quality gears, for which continous mode milling
      might be satisfying enough.
      But don't forget that also hobbing has quite the same problems, since
      a good hob in AA class may be built only in brazed-blade mode,
      needs a proper sharpening,
      and its quality depends upon re-sharpening process too, while
      indexable insert hobs hardly reach quality A and often stop at B.
      Gears milling is then a comparable alternative to hobbing, just
      because both process might lead to a comparable quality.


12     Advantages in gears milling
12.1   * Gear design
      * Every geometric parameter of gear may be dimensioned in
        absolute freedom, without any necessity of follow standard values, up to
        operate even a difference in normal pressure angle of working
        and not-workimg flank, in order to improve stress strenght without
        overloading bushings.
        This kind of freedom is already given by grinfding process too, so
        that couple milling + grinding offers a complete manufacturing process.
      * Module value may be set very large, since milling tool
       dimensions are not very affected by module value (as happens in hobbing).
      * Central gap in double-helical gears may be dimensioned only in
        reference to grinding and milling necessity, that are usually lower tha hobbing ones.
      * Both milling and grinding operate in single-share mode, so that it is
        possible to machine partial toothing, also for pieces that have
        some volumes OVER root diameter.
        Large gears may be machined by sectors, with proper milling paths.
      * All design chances correspond to macxhining opportunities for
        gear manufacturers that work only for other firms, that may face any
        machining request without care about hobs availability.
12.2   * Machine tool (CNC Machining center with rotary table).
      * The machine, also if mainly used for toothing, still owns its
        performances, and may be used as an ordinary machining center over
        other kind of products or other surface on a gear.
      * In case of fast table it is possible to operate turning machining.
      * Machine may be used for a previous check of geametric conditions of gear,
        due to heat treatment for example.
      * The same machine may operate , other than involute cut, also first
        rough machining and/or root fillet machining.
      * With proper CNC software, it is possible to machine also large
        spur bevel gears, for any generating lenght.
        (Available photos on request)
      * Machining of long pinions may be improved by using a rotary
        table with horizontal axe, with edge and intermediate counter-supports.
      * Respect to hobbing machines, speed table in continous milling modes is very
        lower than in hobbing mode, with speed ratio about 60:1 - 80:1
        and table is stopped in ulti-plane mode.
        This means that CNC equipement is very cheaper (Don't forget that any
        supply offer of hobbing machine shows different prices according
        to required maximum table speed!).
      * No tool rotation control is required.
      * In case of machining of pinions with just a few teeth,
        there is non limit to cutting speed.
      * In case of power failure , no damage occours in multi-plane mode
        and low damages occour in continous mode (Anyway less tha in hobbing mode,
        when both hob and gear have high speed at the momento of power failure).
      * Machining center suppliers are quite numerous and behave in correct
        anti-trust mode.
12.3   * Tooling
      * One only milling tool is good for machining a large range of
        modules on both right and left flanks, so that it is not necessary to buy a wide set of tools, and in
        double R/L execution too.
        Although standard milling tools may be used successfully, it is
        possible to design some special cutters for gear milling; they
        would cost a little more than a standard tool, but would cost
        quite a little anyway.
        I am personally sure that any milling tool supplier would be
        very happy to may develop such a new product !!.
      * Delivery time of standard milling tool is very short.
      * Milling tool is very cheap.
        The whole tools  set in milling mode has a cost enormously lower than
        corresponding hobs set, also if properly normalized and carefully
        handled and sharpened.
        Don't forget that brazed skyving hobs must be re-sharpened and
        have a limited lifetime.
      * Tools suplliers are a lot and operate in trade conditions, while hob
        suppliers are just a few.
      * Milling tool is light, may be handled easily and also automatic
        tool change may be used.
      * Milling tool diameter may be quite small since cutting speed is
        easily controlled by rotation speed.
      * All cutting inserts move at the same speed, and in hobs cutting
        speed depends upon insert position over the hob.
      * Milling tool usually takes one only type of insert.
      * A lot of HM qualities and geometries are available.
      * HM inserts for milling are standard, cheaper and offer a greater
        number of cutting edges available.
      * It is possible and fast to change inserts on-board.
      * Milling tool is not required to be as precise as an hob.
      * Not necessary have R/L tools.
      * No re-sharpening is necessary.
      * Also hardened materials may be machined.
12.5   * Machining conditions
      * Cutting action is immediately productive, without initial and
        final partial phases as it happens in hobbing.
        No extra-streoke is required also for large helix angle.
      * Centering of pre-existing surfaces is easy.
      * Cutting speed is undependent and may be set according to HM performances.
      * In case of use of 2 milling tools, machining time may reduce up to 50%.
      * Stock removal is greater than in hob-skyving operation.
      * It is possible to choose different scan policies, in both continuos and multi-plane
        mode.
      * Feed and rotation may be stopped instantly without further problems.
      * Crash consequences are less grave than while hobbing.
      * Machining action is easily in sight.
      * Low table speed permits an easy chips removal.
      * It is not necessary to assure perfect position of gear on the
      rotary table; it is enough to know desplacement vector and consider
      it in additional offset position during machining.
      In continous mode it is necessary to share the path and calculate a proper modified goal
      according to center desplacement.
      In multi cut mode the table is stopped in a well known position
      during single cut and local offset modification is very easy.


13     Machining time
13.1   Continous mode
      In case of gear machininig by continous mode, the milling tool
      runs along teeth profile, from tip circle down to diameter that
      it is necessary to warrant.
      For usual teeth dimensions the lenght of this path is about
      2 - 2,2 x normal module.
      In case it is possible to fit Feed value along X in order to have
      constant feed value along the profile, ([fig15A][fig16A]) according to:

        [15] FEED (X) = FEED profile * Rb / X current

      thus:

        [16] FEED (X) = FEED profile * KFeed  with KFEED = Rb / X

      active maching time for a path-lenght s= 2,2 * module
      may be calculated by:

        [17] Tunit = s / Frel = 2,20 * mn / Frel

      and for the whole gear, consisting in Z teeth cut in L/p levels:

        [18] Ttotal = Tunit * z * L / p = 2,2 * mn * Z * L / (p * Frel)

      In case feed on profile Frel = 150 mm/nin and p = 50 mm will be:

        [19] Ttotal = Tunit * z * (L / 50) = mn * z * L / 3409

      For example, with (Frel=150 p=50) mn=30 z=28 L=500 will lead to 123'
      = 2,05 h for each flank , thus 4,10 h for whole facewidth, that
      might reduce to about 2,50 in case of double tool.
      By using an HM insert hob diam 360 mm , with cutting parameters:
      Vt=110  n=97  a=1,25  L=500+250=750 we have about 173'=2,90 h for
      whole facewidth.
      This may seem a good result, but if you consider all remaining
      service activities (handling, insert change, offset, controls etc)
      and the cost of tool and inserts, I think to may say that milling
      is anyway a convenient way of machining.
      Don't forget that 1 only milling cut may remove much more material
      stock than a HM skyving unit action.
13.2   Multi-plane mode.
      Machining time in multi-plane mode will be a little higher than in
      continous mode, because there are more many not-cutting movements
      and some paths are partially covered each other.
      Only a real test may show the difference, and I extimate machining time in
      multi-plane mode might be about 1,2 * continous mode time.


14     Machining diagram
14.1   Continous milling mode


:    ( 3 levels loop )
: SETTING UP:
: PLOT of tool and gear assembly : verify dimensions
: INPUT DATA of design gear parameters mn,alfa,beta,X,b,da
: INPUT limit curvature radius start-arrive and axial step
: INPUT gear center desplacement error (eventual)
: COMPUTE indexing,rolling and helix parameters
:
:   MACHINING:
:   FOR FLANK = R,L
:     INDEX tool axe = base helix angle
:     COMPUTE offset values due to tool and tool holder
:     FOR AXIAL LEVEL = BOTTOM TO TOP
:       COMPUTE offset values due to helix (eventual)
:       FOR TEETH = 1 TO Z
:         COMPUTE offset values due to gear index
:         COMPUTE total offset values
:         EXECUTE unit cut from r-start to r-end
:          (in case of center desplacement: divide unit cut into
:            fractions with linear approx)
:       NEXT TEETH
:     NEXT AXIAL LEVEL
:   NEXT FLANK
:   END

14.2   Multi-plane mode


:    (4 levels loop)
:  START
:  SETTING UP:
:  PLOT of tool and gear assembly : verify dimensions
:  INPUT DATA of design gear parameters mn,alfa,beta,X,b,da
:  COMPUTE all optimized planning chances from 2 to 8 cuts
:  CHOOSE best cutting plan according to max out-tool
:  INPUT gear center desplacement error (eventual)
:  COMPUTE indexing,rolling and helix parameters
:
:  MACHINING:
:  FOR FLANK = R,L
:    INDEX tool axe = base helix angle
:    COMPUTE offset values due to tool and tool holder
:    FOR PLANNED CURVATURE RADIUS = LONGEST TO SHORTEST
:      COMPUTE gear rotation according to current curvature radius
:      ASSIGN micro-cut parameters
:      FOR TEETH = 1 TO Z
:        COMPUTE offset values due to gear index
:        FOR AXIAL LEVEL = BOTTOM TO TOP
:          COMPUTE offset values due to helix (eventual)
:          (in case of center desplacement: COMPUTE additional
:          offset values)
:          COMPUTE total offset values
:          EXECUTE unit cut cycle
:        NEXT AXIAL LEVEL
:      NEXT TEETH
:    NEXT PLANNED CURVATURE RADIUS
:  NEXT FLANK
:  END


15 Comparision between hobbing and milling

:      Some notes are referred to one only machining mode:
:           ** : referred to milling by continous rolling mode
:            * : referred to milling by multi-plane cuts mode

|                              Technology                                    |
|----------------------------------------------------------------------------|
|           H O B B I N G           |           M I L L I N G                |
|                                   |                                        |
|============================================================================|
|                            gear design                                     |
|----------------------------------------------------------------------------|
| Module value up to 30-35          | No limit to module value               |
|                                   |                                        |
| Maximum diameter related to       | No limit to diameter in case of        |
| machine dimensions                | machining of partial sectors           |
|                                   |                                        |
| Pressure angle must be standard   | Any pressure angle may be machined     |
| Immediate machining only if hob   | Immediate machining of any kind of     |
| is available                      | gear                                   |
|                                   |                                        |
| Teeth must be simmetric           | Teeth may have different pressure      |
|                                   | angle on working and backlash flanks   |
|                                   |                                        |
| Central groove must be wider      | Central groove may be thinner          |
|                                   |                                        |
| Toothing must be possible on      | Toothing may be interrumpted by filling|
| complete 360 degrees tour         | volumes OUT OF root diameter           |
|                                   |                                        |
|============================================================================|
|                             Machine tool                                   |
|----------------------