Feed rate after G0, like G1 X Y F100.

[PcRobotic]

Hello everyone,
   My company just bought 2 brand new YCM machines and the control is FANUC.  However, this control is very picky about between the G0 and G1.  If G0 then it would erase the previous feed therefore at G1 it must have FEED, it cannot remember the previous feed.  Please take a look at the G-CODE of which I have pasted below here. 

 

I truly appreciate for the help, once again thank you for your time to help me out.

 

=======================================

3(.1875, 3/16 EM, CB, USED TOOL,)
(2FLTS .281LOC, .281RLF, .38STO)
G0 G17 G40 G49 G80 G90
G91 G28 Z0 M19(XY STK= .015)
/G28 Y0.(AREA MILL)
T3 M6(ROUGH OUT 2X OPEN SLOTS, CUT#2)
G90 G54 S7500 M3(.0052 -.0094STEPOVER, 5.PERC)
X2.7968 Y-.0215 T4(NEXT TOOL)
G43 H3 Z1.(DOC= Z-.2723 , .2423DP, .015 BROKE THRU)
M8 Z.0625
G1 Z-.1935 F100. ================> GOOD FEED HERE
Z-.197
(CUTTING...)
Z-.1935
G0 Z.125
Y-.0093
Z.0625
G1 Z-.1935 ===========> FEED SHOULD BE HERE AS F100.
Z-.197
X2.7942 Y-.0092 Z-.2139
(CUTTING...)
X2.7942 Y-.0541 Z-.2139
X2.7968 Z-.197
Z-.1935
G0 Z.125
Y.0035
Z.0625
G1 Z-.1935  ===========> FEED SHOULD BE HERE AS F100.
Z-.197
X2.7942 Y.0036 Z-.2139
(CUTTING...)
X2.7968 Y-.0668 Z-.197
Z-.1935
G0 Z.125
Y.0167
Z.0625
G1 Z-.1935 ===========> FEED SHOULD BE HERE AS F100.
Z-.197
X2.7942 Z-.2139
(CUTTING...)
X2.7968 Y-.08 Z-.197
Z-.1935
G0 Z.125
Y.0304
Z.0625
G1 Z-.1935===========> FEED SHOULD BE HERE AS F100.
Z-.197
X2.7941 Y.0305 Z-.2139
(CUTTING...)
X2.7968 Y-.0938 Z-.197
Z-.1935
G0 Z.125
Y.0451
Z.0625
G1 Z-.1935===========> FEED SHOULD BE HERE AS F100.
X2.7967 Z-.197
X2.7941 Y.0452 Z-.2139
(CUTTING...)
X2.7968 Z-.1935
G0 Z.125
Y.0611
Z.0625
G1 Z-.1935===========> FEED SHOULD BE HERE AS F100.
X2.7967 Z-.197
(CUTTING...)
X2.7968 Z-.1935
G0 Z.125
Y.0795
Z.0625
G1 Z-.1935===========> FEED SHOULD BE HERE AS F100.
X2.7967 Z-.197
(CUTTING...)
X2.7968 Z-.1935
G0 Z.125
Y.1024
Z.0625
G1 Z-.1935===========> FEED SHOULD BE HERE AS F100.
X2.7967 Z-.197
(CUTTING...)
X2.7968 Z-.1935
G0 Z.125
X2.7967 Y.1535
Z.0625
G1 Z-.1935===========> FEED SHOULD BE HERE AS F100.
Z-.197
X2.794 Y.1537 Z-.2139
(CUTTING...)
X2.7967 Z-.1935
G0 Z.125
X2.6157 Y-1.5659
Z.0625
G1 Z-.1935===========> FEED SHOULD BE HERE AS F100.
X2.6158 Z-.197
(CUTTING...)
X2.6269 Y-1.5557
Z.0625
G1 Z-.1935===========> FEED SHOULD BE HERE AS F100.
Z-.197
X2.629 Y-1.5574 Z-.2139
(CUTTING...)
Y-1.2256 Z-.2722
G3 Y-1.1503 Z-.1935 R.0787
G0 Z1. M9
G91 G28 Z0.
/G28 Y0. M5
G0 G90 G54 X0.
M1

[Zaffin_D]

Download the latest MPFan from Mastercam's tech exchange.  In it there is a switch for this.

[So not a Guru]

I would think that you might be able to change that behavior thru the Fanuc parameters.

[Leon82]

It is one of the modal group parameters probably group 01 or 02. 

 

The yellow book has all the parameters listed in each group

[crazy^millman]

On 11/20/2018 at 3:03 AM, So not a Guru said:

I would think that you might be able to change that behavior thru the Fanuc parameters.

Yes fix the machine and have it act like every other Fanuc on the planet.

[PcRobotic]

On 11/20/2018 at 2:26 AM, jeff.D said:

Download the latest MPFan from Mastercam's tech exchange.  In it there is a switch for this.

Hello Jeff,
   I downloaded and it works fine,  and I would like to know which is the switch name so I can find out.  Do you remember the switch name, so I can study about it Jeff?


Thank you.

[PcRobotic]

On 11/20/2018 at 3:03 AM, So not a Guru said:

I would think that you might be able to change that behavior thru the Fanuc parameters.

Sadly, the company think machinists are superman who can do everything.  I have asked and they said "YOU FIGURE IT OUT..."... The only way is to trick in the post.

[PcRobotic]

3 hours ago, 5th Axis CGI said:

Yes fix the machine and have it act like every other Fanuc on the planet.

Thank you, 5Th Axis.  Insanely I have to ask people around because YCM demand to charge money whenever they trouble shoot something at the control and the thing is my company won' spend a dime on that because they thought everything is PERFECT as it is BRAND New.....

[crazy^millman]

1 hour ago, PcRobotic said:

Thank you, 5Th Axis.  Insanely I have to ask people around because YCM demand to charge money whenever they trouble shoot something at the control and the thing is my company won' spend a dime on that because they thought everything is PERFECT as it is BRAND New.....

This is a warranty item in my opinion not a chargeable item. They are not willing to fix for free then tell them to come get the machine at their cost since it is not meeting specifications. You can give them my number as your SME (Subject Matter Expert) and I will be glad to help them understand why they should want this to work correctly.

[Leon82]

Look up the parameters in the 3200 range in the yellow fanuc book. These parameters are  in groups and modality is determined by the parameter setting. There are quite a few but the book says which are in what group.

[Newbeeee™]

12 hours ago, PcRobotic said:

Sadly, the company think machinists are superman who can do everything.  I have asked and they said "YOU FIGURE IT OUT..."... The only way is to trick in the post.

Can you not send an email to the company that supplied the machines and ask them yourself - ignore the idiots in the office?

You need the machines to behave like all the other machines in your shop so you can put already programmed jobs onto these new machines.

It will only be a parameter change.

[Leon82]

It looks like it's parameters 3406-3409.

 

I think it's page around page 2800

[PcRobotic]

Hello everyone,
   First of all, thank you for the BIG HELP and here is what I found out from MPFAN.  

 

Add this...
# --------------------------------------------------------------------------
# General Output Settings
# --------------------------------------------------------------------------
force_feed   : yes$  #Force output of feed rate on first feed move following rapid motion?

#Region pRapidOut
prapidout       #Output to NC of linear movement - rapid
      sav_gcode = gcode$
      if convert_rpd$ = one,
        [
        gcode$ = one
        feed = maxfeedpm
        ipr_type = zero
        ]
    #"DEBUG: ", ~mr3$, ~nextop$, e$
      if tool_op$ = 19, "M0(AGAINST PIN STOP HERE)", e$
      
      pcan1, pbld, n$, sgplane, `sgcode, [if gcode$ = 1, sgfeed], sgabsinc, pccdia,
        pxout, pyout, pzout, pcout, [if gcode$ = 1, `feed], strcantext, scoolant, e$
    [
     if (opcode$ > 0| opcode$ < 6),
      if (nextop$=1003 | (nextop$=1011 & t$<>abs(nexttool))),
        "", else, e$
    ] # NO NEW LINE, COOLANT M9
     if force_feed, result = force(feed)  # Force output of feed next time it's called for output, FEED RATE AFTER RAPID  ================ Add this line also