Results 1 to 4 of 4

Thread: Machine or Software Issue? Major Problem

  1. #1
    Join Date
    Sep 2016
    Location
    Eastern Virginia
    Posts
    82

    Default Machine or Software Issue? Major Problem

    Yesterday things worked fine. Today, not. I tried to cut a toolpath after I had gotten a new bit. I entered the bit in the DB just like others. Saved the toolpath just like others. The material setup is at 0,0 datum. The preview shows it perfectly. The actual piece, not. I had cut this exact same toolpath before, with a different bit, no problem.

    1. The spindle did not turn on - it was turned on at the machine, but when I ran the cut it did not come on. I didn't know it because of the dust boot and vac noise until after. Note - the spindle came on and ran fine during the warmup routine just before.

    2. The 0,0 points were not the same. Software was at bottom left corner. What actually happened looked like something, either software or machine, thought X,0 was in the middle.

    3. I had X,Y zeroed the machine to the bottom left corner before running the cut.

    4. The red diagonal line in the preview is because I have my machine set to return to the middle of the cutting area, and that's also where it starts.

    Pics attached (can't attach g code). Baffled.

    nsbad.jpgnspreview.JPG
    ShopBot Desktop 24x18
    Spindle
    VCarve Pro 8.5xx
    ScottP Super Deluxe Spoilboard

  2. #2
    Join Date
    Sep 2016
    Location
    Eastern Virginia
    Posts
    82

    Default

    Since I can't post the code, here's at least the top part of the file. I'm using Shopbot version of V Carve Pro 8.514 with the Shopbot post proscessor, no mods.

    '----------------------------------------------------------------
    'SHOPBOT ROUTER FILE IN INCHES
    'GENERATED BY PARTWorks
    'Minimum extent in X = 0.000 Minimum extent in Y = 0.000 Minimum extent in Z = -0.625
    'Maximum extent in X = 12.000 Maximum extent in Y = 5.500 Maximum extent in Z = 0.000
    'Length of material in X = 12.000
    'Length of material in Y = 5.500
    'Depth of material in Z = 0.625
    'Home Position Information = Bottom Left Corner, Material Surface
    'Home X = 12.000000 Home Y = 10.000000 Home Z = 1.700000
    'Rapid clearance gap or Safe Z = 0.200
    'UNITS:Inches
    '
    IF %(25)=1 THEN GOTO UNIT_ERROR 'check to see software is set to standard
    SA 'Set program to absolute coordinate mode
    CN, 90
    'New Path
    'Toolpath Name = V-Carve NS 60 1-4 010 tip Ons
    'Tool Name = 1/4" 60* 010 tip Ons ENGRAVING 37-03

    &PWSafeZ = 0.200
    &PWZorigin = Material Surface
    &PWMaterial = 0.625
    '&ToolName = "1/4" 60* 010 tip Ons ENGRAVING 37-03"
    &Tool =35 'Tool number to change to
    C9 'Change tool
    TR,18000 'Set spindle RPM
    C6 'Spindle on
    PAUSE 2
    '
    MS,0.7,0.4
    JZ,1.700000
    J3,2.351121,3.642589,0.200000
    ShopBot Desktop 24x18
    Spindle
    VCarve Pro 8.5xx
    ScottP Super Deluxe Spoilboard

  3. #3
    Join Date
    Sep 2016
    Location
    Eastern Virginia
    Posts
    82

    Default

    For future reference, Support fixed it quickly. Thank you. It was because I had the bit as number 35. It seems I can only have bits numbered 1-19 in my current setup. Here is the complete answer:

    The ShopBot software uses tool numbers to define which cutting head you are using. Cutting head number 1 (what you have) uses number 1-19 for tool numbers. Since you selected tool 35 you were telling the tool that you were using cutting head number 2 which uses a different output to turn the spindle on (which is why your spindle didn’t come on) and has an offset (which is why it didn’t cut in the right location)
    ShopBot Desktop 24x18
    Spindle
    VCarve Pro 8.5xx
    ScottP Super Deluxe Spoilboard

  4. #4
    Join Date
    Apr 2007
    Location
    Marquette, MI
    Posts
    3,388

    Default

    Walt...
    You may have omitted a viable option: User Error. Which may be the case in this instance.

    If the ShopBot TC custom files work today the way that they have in the past, tools that are designated to be run in Head 1 (main Spindle or Router) should be numbered #1 thru #19. Using a tool number outside of that range, will not switch on the router/spindle.

    Using a tool #35 would have plunged and turned on drill 1 if one is present. Code from the Header of the "MTC" file pasted below.


    'MTC.SBP
    'Manual Tool Change Handler // Parallels ATC System
    'For Use with PartWorks Posts for Manual Tools Changes
    '5/2/10
    '
    'Head 1 (Z) tools are #1...#19
    'Head 2 (A) tools are #21...#29'
    Drill 1 (Z) tools are #31...#39
    'Drill 2 (Z) tools are #41...#49
    'Drill 3 (A) tools are #51...#59
    'Drill 4 (A) tools are #61...#69
    Gary Campbell
    GCnC Control
    GCnC411(at)gmail(dot)com
    Servo Controller Upgrades
    http://www.youtube.com/user/Islaww1


    "We can not solve our problems with the same level of thinking that created them"
    Albert Einstein


Posting Permissions

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