Unexpected tool path when using TNR

[gibsoni]

Hi Guys,

I would greatly appreciate some help with my OSP7000 control.

Im working inside the bore of a hollow part and prior to parting off, I chamfer the inside corner.

I make a clearance groove and then put a radius on the created corner.

I am now unable to make the control do this for some reason.

I have TNR P value set to 1 and 0.4mm rad for X and Z.

The radius is not where it should be on the animation and appears to be the wrong rad.

When I change the TNR values to '0' its all fine in terms of tracing animation - but of course the geometry will be wrong without TNR comp.

Section of program below - Z0 is at the parting plane.

Thanks for any ideas as to where I am going wrong.

Iain.

(INTERNAL CHAMFER)
T170717
G96 M03 S30
G00 X45.0 Z65 M08
G00 X45.0 Z0
G01 X50.5 Z0 F.05
G00 X45.0 Z0
G00 X45.0 Z2
G41
G01 X47.5 Z1 F1
G02 X49.5 Z0 I1 F.05
G00 X40 G40 I-5
G00 Z100

Similar Threads:

• Help with an unexpected program tool move
• Mach3 unexpected plunge after tool change
• G Code Generating Unexpected Tool Path
• Solved V25 - Unexpected clipping in tool path
• Need Help!- Rotory tool path is posting out new cord with every path?

[deadlykitten]

hi, pls share tool geometry, drawing before and after the operation / i will give you code

ps : i know, Z0 at left of the part

[gibsoni]

Hi Deadly Kitten,

Thanks for your offer to help (Again :-) )

Ive attached a drawing of the rad I want to machine, breaking the internal corner before parting off.

The tool is a 4mm grooving tool with 0.4mm radius. Obviously calling the RHS edge of the tool as operator looks at it.

Code I am using is in the earlier post.

Regards, Iain.

[deadlykitten]

hi gibsoni there is a problem with rad comp toolpaths that begin or end with an arch

there are 2 codes in this post :
... 1st code uses radius comp
... 2nd code uses only coordinates
*it took me few seconds to create the 2nd code, and i spent some time debuging the 1st code

about the 1st code :
... normally, the line " Z1 " should not be there, but is critical to be there
... also " G01 X0 G91 " is a trick that should not be there
... it should work without the imaginary vector, but i couldn't make it work without it
* the code works, but is a tiny mess

long live Okuma / kindly

ps : speed is changed from 30 to 250 M/min; i don't have all day also, it may be too much effort to cut with that big insert at the interior; maybe you should consider an insert of only 3 or 2.5 mm ? 4 seems big ...

    G50 S2000
    G00 X500 Z200

    T+01*10101                ( w4r0.4p1 )
    M61
    G96 M03 S250 M08
    G00 X45   Z65
              Z0
    G01 X50.9      F0.05  G95 ( 47.5+2*1+2*nose_radius+0.6_clearance )
        X-0.4             G91
    G00 X45               G90
              Z1
    G01 X47.5      G41 K1     ( imaginary vector for positioning among a tangent at angle 0 )
    G02 X49.5 Z0       I1
    G01 X0                G91
                   G40    G90
    G00 X45
              Z100

    M02

    G50 S2000
    G00 X500 Z200


    T+01*101                     ( w4r0.4 )
    M61
    G96 M03 S250 M08
    G00 X45      Z65
                 Z0
    G01 X50.9         F0.05  G95 ( 47.5+2*1+2*nose_radius+0.6_clearance )
        X-0.4                G91
    G00 X45                  G90
    G01 X2*23.75 Z1.4
    G02 X2*25.15 Z0   I1.4
    G00 X45
                 Z100


    M02

[deadlykitten]

hello, both codes from previous post work, thus they deliver the part

problem is that they deliver only that part, while another part will require another code

... and this is where parametric codes kick in

only for this type of operation, pls find in attached image, 3 kind of toolpaths :
... right : clearance groove + radius
... middle : clearance groove + radius approach + radius ( this code will smooth out the entrance of the tool )
... left : clearance groove + chamfer + radius approach + radius ( this code will smooth out the entrance of the tool and will reduce cutting effort when cutting the radius )


same operation can be coded anywhere between " speed " and " longer tool life & reduce cutting effort "

each type of toolpath requires a different execution time and has different stability

if you wish to increase specs, then you need to start with a stable smooth toolpath, so to eliminate sudden effort peaks that may stress the cutting edge

next code is a parametric approach for the "right" image / kindly

    G50 S2000
    M61


  ( back internal radius / etc )


    NOEX V1 = 47.5  ( id           )
    NOEX V2 = 1     ( radius       )
    NOEX V3 = 0.4   ( nose radius  )
    NOEX V4 = V1-3  ( id clearance )
    NOEX V5 = 70    ( Z  clearance )


  ( * )


    G00 X500 Z200


    T + tool_post * 101                          ( w?r? )
    G96 S M42 M03 M08
    G00 X+V4               Z+V5
                           Z0
    G01 X+V1+2*[V2+V3+0.3]         F      G95
        X-0.4                             G91
    G00 X+V4                              G90
    G01 X+V1               Z+V2+V3
    G02 X+V1+2*[V2+V3]     Z0      I+V2+V3
    G00 X+V4  
                           Z+V5


    M02

[deadlykitten]

one more thing : you have declared P1 for that tool; why ?

[deadlykitten]

there is a problem with rad comp toolpaths that begin or end with an arch

hello there is a trick to handle this; i discovered it today, by checking a program created by someone else, for attached toolpath ( dimensions does not matter )

it works, but i don't understand why the controller hits a wall when it must deal with comp and arches at toolpath end, and i don't understand the solution ?! kindly

    G00 XA ZA G42
    G01 XB ZB
    G03 XC ZC L
    G01       G40 ( if G01 is removed, code will fail )

[kurmay]

Cancel of TNRC isn't possible when circular interpolation (G2 or G3) on OSP controller.
Maybe it is same on RS274NGC too.

[deadlykitten]

hi kurmay, i was told that that code was generated by igf

i asked because that particular solution could not have been generated by any cam post

in other words, okuma guys are aware of this, and they solve it by g01 g40 combo ( without using coordinates )

inside the manuals, there is no block that contains only those 2 codes

problem & solution, are both weird; i don't believe i would have guessed it / kindly