Dialog4 Parameter Programming Question
Close
Login to Your Account
Results 1 to 5 of 5
  1. #1
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    685
    Post Thanks / Like
    Likes (Given)
    880
    Likes (Received)
    131

    Question Dialog4 Parameter Programming Question

    Anyone here know if you can use Parameter formulas/calculations, in blocks between G41/G42 (start of tool compensation) and G40 (end of tool compensation? I know you can use simple parameters inside those blocks, but am having issues with formulas that are written inside tool compensation blocks.

    Not seeing any discussion of this in the Dialog4 parameter manual and none of the examples show formulas inside tool comp, only in blocks before or after tool comp.
    Last edited by Colt45; 10-10-2019 at 07:47 PM.

  2. #2
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,022
    Post Thanks / Like
    Likes (Given)
    1793
    Likes (Received)
    2372

    Default

    Don't have an answer, sorry. Eons since i used the Parameter programming features....CAM system sort of negated the need.
    Believe that there are features of the parameter programming that don't appear in the supplemental programming manual.

    Some time back Martin posted about features that were not in the manual.Things he picked from Euro forums...ways to enter different values in different locations within a block .
    Might do a search to see if anything there has value for your question.

    See: Parameter problem

    Would like to see your code....

    On edit, just looked at the "software Update" booklet for Dialog 4 and within the section on parameter programming there are examples of calling "P" values within a compensated (G41/G42) moves....
    (programming example #3 page 1-32)

    Looks to be compound "P" values used there with math operations ...Did not spend too much time with this, but looks like the pocket is cut with a tapered wall where the cutter path is changed as it steps down,
    Sort of cute...
    Cheers Ross

  3. #3
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    685
    Post Thanks / Like
    Likes (Given)
    880
    Likes (Received)
    131

    Default

    $%9998

    t1 r0.0625 a l a

    p1 =1.0
    p2 =0
    p3 =0
    p4 =((p1:2):0.86602)
    p200 =(p2+p5*p4)
    p300 =(p3+p6*p4)



    %
    ($%9998/000000"hex via parameter)
    n1 g17 t1
    n2 z1 f35.0 s+1250
    n3 g0 x0 y0 c0
    n4 z0.1 f10.0
    n5 p5==0.5
    n6 p6==-0.8660
    n7 x= p200 y= p300
    n8 p5==-0.5
    n9 p6==-0.8660
    n10 x= p200 y= p300
    n11 p5==-0.8660
    n12 p6==0
    n13 x= p200 y= p300
    n14 p5==-0.5
    n15 p6==0.8660
    n16 x= p200 y= p300
    n17 p5==0.5
    n18 p6==0.8660
    n19 x= p200 y= p300
    n20 p5==0.8660
    n21 p6==0
    n22 x= p200 y= p300
    n23 p5==0.5
    n24 p6==-0.8660
    n25 x= p200 y= p300
    n27 g0 z1
    n28 m30
    ?
    0000

    Something happened to my formatting when I pasted this into the forum- all the letters changed from upper case to lower case.
    Program runs perfectly on my FP4NC, when I try to add tool compensation via G41/G42 I get error messages and it won't run.

    This is a program to machine a hex- "P1" is the inscribed circle of the hex flats.
    We use "P" values with compensation on (and also inside canned cycles) every day, the issue here is "calculations/formulas" inside compensation.
    Would like to run tool comp to adjust the finished size of the hex and also apply G7 to the outside corners.
    Tool comp would also allow this program to make either internal or external hexes just by changing which side of the hex the tool is on via G41 or G42.
    Last edited by Colt45; 10-11-2019 at 09:49 AM.

  4. #4
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,022
    Post Thanks / Like
    Likes (Given)
    1793
    Likes (Received)
    2372

    Default

    Steve:
    Funny, but i wrote this hex milling program some years back....bit of digging and this is what i have on this.

    N1 G0 X0.0 Y0.0 Z4.0
    N2 G17 T1*1
    N3 S= P6
    N4 G0 Z.1 M70
    N5 G91 Z = -P13 F= P4 M70
    N6 G90 M70
    N7 G41 G47 A= P7 X= P10 Y= -P11 G0 G64 G61
    N8 X= -P10 F = P5
    N9 G7 R= P12
    N10 X = -P9 Y 0.0
    N11 G7 R = P12
    N12 X= -P10 Y= P11
    N13 G7 R= P12
    N14 X= P10
    N15 G7 R= P12
    N16 X= P9 Y 0.0
    N17 G7 R= P12
    N18 X= P10 Y= -P11
    N19 G7 R= P12
    N20 X 0.0
    N21 G40 G47
    N22 G91
    N23 G0 Z.1
    N24 G90
    N25 L= P14 N5 N24
    N26 G0 Z.1
    N27 T1
    N28 L1 N5 N26
    N29 G0 Z4.0
    N30 G0 X0.0 Y0.0
    N31 M30




    P list (mode 12)

    P1= (Hex size , across flats given in inches)
    P2= (Height of hex in inches)
    P3= (number of depth passes to get full height)
    P4= (feed rate for depth moves) Note: rate will be 1/10 of value entered here
    P5= (Feed rate around profile) Note: rate will be 1/10 of feed rate entered here
    P6= (+Spindle speed)
    P7= (enter value for arc out and arc into contour)
    P9= P1* .5774
    P10= (P1*.5774) / 2
    P11= P1 / 2
    P12= P1 / 8 (this setting makes the corner radius as a percent of the hex size, shown as 1/8 the hex size here)
    P13= (P2 / P3) + .100
    P14= P3 - 1

    Some explanation:
    P1 is the size of the hex you wish.
    P2 is eh height of the hex.
    P3 is the number of cuts needed around the profile to get to full depth.

    The program cuts the profile to depth then calls a finish tool for final passes around the part.
    Hex is oriented with the starting flat parallel with the "X" axis)
    Corner radius is a function of the hex size...can set that amount in "P" 12.
    Profile cuts are retracted at the end of the profile before reposition and next depth cut.
    Depth moves are done incrementally, so it might be possible to have accumulating errors if lots of passes are needed to get the depth...

    As with anything, might be errors in typing this so proof the program and use at your own risk..

    T1*1 is the rough cutting tool. Call cutter radius larger than the true size of the tool by the amount needed for finish cut.
    T1 is the true size (radius) of the tool.
    Both rough and finish cuts done with the same actual tool.

    Cheers Ross
    Last edited by AlfaGTA; 10-15-2019 at 10:48 AM.

  5. Likes Mud, Colt45 liked this post
  6. #5
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    685
    Post Thanks / Like
    Likes (Given)
    880
    Likes (Received)
    131

    Default

    Too funny, I got the idea from reading one of your old posts!
    I was able to get this to work, simply a matter of getting G41/G42 in the correct block, in this case, following N4.
    Will cut internal or external hex, depending on whether G41 or G42 is used.
    Thanks for the follow up-cheers!


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •