Machine or Software Issue? Major Problem

[Walt_S]

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.

2957029571

[Walt_S]

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

[Walt_S]

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)

[Gary Campbell]

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