Posting (arc fit box) and G19 issue

BobCAD-CAM Software Discussions
#1

I just started using the Arc fit check box for 3 axis milling and I just ran into an issue where it put one G19 in the code because of checking arc fit box. this changed my axis and the next operation was a drill. It went into the hole and immediately started to move in the x axis and started pecking in the Y. well it would have if it didn’t stall the machine out. Anyone else have this issue? this was on a Haas vf6 3 axis mill and Bobcad version 33

#2

I click the box all the time. On my Haas’s and have never had any issue. Maybe you have a bad post?

#3

Yeah it is probably in the post. the weird thing is that it didn’t put the g19 at the beginning or end but somewhere in the middle of the 3d. I was using 3 axis advanced Z level finish when it did a g19. I had a bunch more 3d that ran after that then the drill came up and did the crash. I have been using this post for many years now but just started trying the arc fit box.

#4

I use arc fit alot, for the obvious reasons of having less code and better finishes. Occasionally when it needs it will use G18 or G19 and not post the G17 when it posts toolpath that is in the xy plane. There must be something in the post that needs to be done in order to have the right g plane code be posted.

Anybody know ?

Thanks
David.

#5

I have my G17 at the top right after the tool change as part of my safe blocks on all tool changes if it don’t need it it will just be fine.

#6

OK Eric this is what i think i need to do to my post to fix the issue. ill start going thru it to find out where to put it in. If you know what im looking for in the post that would be awesome.

#7

I do the same, G17 at tool changes. However if the tool is doing multiple features and it use G18 or G19 in one and not all, that is where I would have to manually edit it in. I guess I could have a G17 output at the beginning of each feature to take care of that.

If the g codes for the xy, xz yz planes can be modal, then the system should post automatically when the tool plane changes from one plane to the other.

The NC Editor is good at catching things like that.

David.

#8
  1. Tool change
    MDI_BeforeToolChange
    n,t
    n,rapid_move,incremental_coord,“G28”,“Z0.”
    n,optional_stop
    n,“G00”,“G17”,“G40”,“G49”,cancel_drill_cycle,measure_mode,movement_mode
    " "
    “(NEXT CUT - NEXT TOOL)”
    system_comment
    feature_name_comment
    MDI_AfterToolChange
    " "
    “(TOOL #” ,list_tool_number," ", tool diameter, tool_label, “)”
    n,t,“M06”
    n,coolant_on
    output_rotary_angle
    n,“G00”,absolute_coord,work_coord,force_x,xr,force_y,yr, p_rot, s_rot, s,spindle_on
    n,rapid_move,length_offset,d_offset,zr,
1 Like
#9

awesome Eric. I just updated my post to do the G17 after every tool change now. Thanks for all the help from everyone

#10

avocamfg2006 I just read over your post and I thought that might also be an issue, so on my machine post it says “next cut same tool” at that line I also will put a G17 just in case. hopefully this works.

1 Like