Fanuc #2005#1 Feed Foward Question / Probing

I had a Renishaw probe installed on a Kitamura VMC w/ Fanuc 16i-MB control a few years back. Recently we purchased the Renishaw Productivity + add-on for our machine and I'm trying to get that up and going. I had to dig around for the specifics on the probe turn-on commands and need a bit of clarity on before I move forward.

The installer set up our Spindle Probe and tool setter to turn on/off with M21/M22 & M23/M24. The programs assigned to those simply flip #1107 and ##1106 between 1 and 0 for On/Off function. (I do have a question on that--but haven't researched yet to make sure what that's doing specifically. I probably can figure that one out, but if anyone wants to save me some time and explain what #1107 and #1106 on/off would be tied to--feel free!) I have verified that those functions are all that is needed to turn the probe and toolsetter on/off.

However, as part of the Spindle Probe turn on Macro command (not the tool setter), the installer also manually entered parameter change codes for variable 2005 as follows:
G10L50
N0020(R04)(PORT CHG TO CARD)
N2005P1R11000000
N2005P2R11000000
N2005P3R11000000
G11

It is not changed back during the probe turn off command, but our M6 routine DOES have the flip back as part of it--as well as another Probe OFF command for each:
#1107=0(SP PROBE OFF)
#1106=0(TS OFF)
G10L50
N0020R05(PORT CHG TO NETWORK)
N2005P1R11000010
N2005P2R11000010
N2005P3R11000010
G11
G10L50
N2005P1R11000010
N2005P2R11000010
N2005P3R11000010
G11

I seem to recall suggesting that we put the port change for the network in the M6 because I knew our users would forget--and I suggested doubling up on the Probe OFF commands there just in case someone left the probe on. I cannot, however, determine what the 2005 commands are doing and the reasoning/purpose behind them. I can assume that they're necessary for the probe functioning properly and make sure I add them in the Productivity+ routines, but I'd rather move them over to the Probe ON/OFF M-Codes because, to me, that's the more proper place for them and I can reference the same M code from Inspection+ and Productivity+ and not end up with some mismatch.

Can someone shed some light on the Feed Foward function on bit 1 and why it may need to be disabled for probe usage?

I appreciate any education/guidance anyone can provide. Thanks!

In a nutshell, #1107 and #1106 are F addresses in the PMC ladder logic. Your M-codes (M22/M23) and (M23/M24) are probably doing the same thing as setting #1106 & #1107 to =1 for on and =0 for off. This allows the program to change the state of the probe without M codes. If you search the PMC ladder for F54.6 (#1106) and F54.7 #1107) you will find how this is being done. I can't think of a reasons why they are disabling the Feed Forward function during probing. You might experiment to see why. I also don't understand why you have to change the port setting (parameter 20). Are you sending data somewhere outside the machine?

Yes, the M21-M24 programs simply flip the #1106 or 1107 and they do actually turn on/off the probe and tool setter. I just wasn't aware what that actually was doing since I couldn't readily find information on those variables. I'll check the PMC ladder in a bit.

The port changing was actually done by me. Our machine can't output probe data via DPRNT over the network interface, but it is how we load/unload all of our programs. I didn't want the operators having to change back/forth all the time, so I put the port change to the Flash Card output into the Probe On command--and had it switch back to the network card during any tool change. I've had a few times where they tried to load a program immediately after using the probe and it was easier to me just tell them to do a tool change than it was to tell them how to edit the output port, etc.

I thought I had came back on here Saturday and posted that I did figure out that the feed forward function was actually part of Renishaw's suggestions in their programming manual (not the installation manual). Per their suggestion:

P2005.1=0 (FEED) If this is set to =1, severe bumping can occur during probing moves. This parameter bit must be set for each axis – X, Y and Z. If the highspeed machining option is not used, it may be possible to turn this parameter off, otherwise it will be necessary to turn it off just for probing and then back on afterwards, under program control.

So that does explain WHY the function is getting turned off and then back on. I'll make sure it's part of the probe turn on M-code as opposed to the start cycle. It seems safer that way. Then I'll reference the M code from the Production + routines to make sure it's done as well.