Inverse time on Matsurra MAM72-35V

[GPC_CNC]

Hey guys,

 

I'm programing some 5x surfacing (parallel to surfaces) on a Matsurra MAM72-35V w/fanuc 30i control.

 

First off, I do understand G93 and how it works. The problem I'm having is that I am maxing out the the feed (the mach def is set to the correct max of 9999. which is the most the machine will accept). The machine has a 20k spindle and I am surfacing some small rads with an 1/8 ball mill at 60ipm which is a lot slower than I would normally surface at using a conventional 3X surfacing path.

 

So that being said I have 2 things I'm concerned with. One, The post will do G93 and then post a feed of F9999. on the first move line and all following lines do not have a feed (shouldn't there be a feed output on every line regardless?) and two, will I get some variation of feed between moves depending on the vector length between moves. Also,I'm doing 60ipm now, but when I drop it to 15ipm I still get a lot of maxed out area's. In other words at 15ipm, I'm going as fast as at 60ipm. I've tried making tolerances, etc. larger to eliminate some code, but I'm still maxing it out in a lot of areas and the areas that aren't maxed are higher in the range. I had always been told that you wanted to avoid being at the max feed on these paths to avoid studdering, or erratic feed fluxuations, etc.

 

Is this normal? I guess I'm used to seeing video's of these machines swinging around at what appear to be very high feed rates. I feel like there should be a big difference in coded feed if I'm programmed at 60ipm vs 600ipm, which it seems that in this case there would be no difference. I certainly feel that at 15 ipm I shouldn't be maxing out any feed rates.

 

Thanks

 

Greg

[YoDoug®]

Mastercam allows you to set wether Inverse is calculating in minutes or seconds. I believe there is also a parameter in a Fanuc for the same. You could be seeing a combination of the setting between Mastercam and the machine that are not doing an "apples to apples" feedrate.

[djstedman]

I am pretty sure that your rotary shouldnt be maxing out when its commanded to go 15 IPM either.

 

If the Max feedrate the machine will take in G93 is F9999. then it seems like unless there is a machine parameter you can change its not going to change much if the code is hitting that F9999. limit regardless what IPM you command in Mastercam.

 

As for should it put out a feedrate on every line.. it is most likely just trying to conserve code.. ie.. it knows the max feedrate according to the control def / post is F9999. so it posts it once and doesnt bother putting in a feedrate slower unless it finds a place where it is actually commanded to go slower than that, an unnescssary F9999. on every line in a 25000 line program is a lot of wasted CNC memory.

[GPC_CNC]

Mastercam allows you to set wether Inverse is calculating in minutes or seconds. I believe there is also a parameter in a Fanuc for the same. You could be seeing a combination of the setting between Mastercam and the machine that are not doing an "apples to apples" feedrate.

 

I just poured through the fanuc encyclopedia and couldn't find anything to set it to seconds. Doesn't mean there isn't one, but I'll probably need to call the apps guy on that.

 

Thanks

 

I am pretty sure that your rotary shouldnt be maxing out when its commanded to go 15 IPM either.

 

If the Max feedrate the machine will take in G93 is F9999. then it seems like unless there is a machine parameter you can change its not going to change much if the code is hitting that F9999. limit regardless what IPM you command in Mastercam.

 

As for should it put out a feedrate on every line.. it is most likely just trying to conserve code.. ie.. it knows the max feedrate according to the control def / post is F9999. so it posts it once and doesnt bother putting in a feedrate slower unless it finds a place where it is actually commanded to go slower than that, an unnescssary F9999. on every line in a 25000 line program is a lot of wasted CNC memory.

 

I was under the impression that a feed code was required under every move block regardless, or maybe it seems that way since most code changes every line when it's not maxed out.

 

Thanks

 

Greg

[Jayson Kramer]

Were did the post come from. that machine will move WAY faster then that.

You should not be getting this inconsistent fluctuation in the cutting. I am taking you folks did not buy the Camplete setup with this machine with the proven post setup. this what I have used in the past.

[GnoGueyJose]

We don't use Inverse on our MAM's. We use CAMplete and Feedrate leveling. It's better all the way around. More control over axis velocity and none of the Inverse Limitations.

 

 

[Chris In-House Solutions]

Hey GPC_CNC

 

I believe you are seeing the F9999. due to the post not being updated properly. There are some parameters that were changed in previous versions and if they are not updated then the post outputs a F9999. How long have you had this post for? Do you know who wrote your post? Do you know who updated your post if it was updated?

[GPC_CNC]

Were did the post come from. that machine will move WAY faster then that.

You should not be getting this inconsistent fluctuation in the cutting. I am taking you folks did not buy the Camplete setup with this machine with the proven post setup. this what I have used in the past.

 

The post came from MPPOSTABILITY. We had the Camplete, but lost the key (stolen?) and a new key is about $15k. Since I don't pay the bills, the decision was made to get a post instead. I did a dry run on the machine that didn't seem to run too badly. I'm just surprised that I would max it out so easily.

 

We don't use Inverse on our MAM's. We use CAMplete and Feedrate leveling. It's better all the way around. More control over axis velocity and none of the Inverse Limitations.

 

See above about camplete, but it sounds like I'm really missing out not having it. Am I simply hitting the limitations of inverse time?

 

Greg

[GPC_CNC]

Hey GPC_CNC

 

I believe you are seeing the F9999. due to the post not being updated properly. There are some parameters that were changed in previous versions and if they are not updated then the post outputs a F9999. How long have you had this post for? Do you know who wrote your post? Do you know who updated your post if it was updated?

 

This is an MPPOSTABILITY post that we got early last year (Feb/March maybe). I believe it came for X5 and we updated it in house when we upgraded to X6. Either way the control def is marked MMD-6. Not sure how to check the post, but I'm pretty sure I updated it all at the same time.

[GnoGueyJose]

That's too bad about loosing your CAMplete key. That's a BS policy having to re-buy the software if you loose a key or it gets stolen. I mean if there's a Police Report or a letter from the CEO/President of the company attesting to it's disappearance, that should suffice and you should get a new key for a nominal fee (to cover the paperwork, cost of the new key, time, etc... - like $250~$300).

[Chris In-House Solutions]

Hey Greg, the post should be good not sure why you are seeing F9999. Those parameters in the post were changed between X2 and X3 I believe. I thought the post was a little older which is why I asked how old the post was.

 

Not sure if this has been covered yet but in your control definition are you sure you have the feedrates set to output Inverse Feed?

[gcode]

this is from an mpgen 5X post..

but I'm sure your post has something similar, hopefully

where you can see it.. and not buried in the binary file.

 

maxfeedpm : 500 #Limit for feed in inch/min

maxfeedpm_m : 10000 #Limit for feed in mm/min

maxfrinv : 999.99 #Limit for feed inverse time

fix_fr : 1 #If feedrate is zero, apply these values

deffeedpm : 1. #Default for zero feed in inch/min

deffeedpm_m : 25. #Default for zero feed in mm/min

deffrinv : 9999 #Default for zero feed inverse time

[GPC_CNC]

Hey Greg, the post should be good not sure why you are seeing F9999. Those parameters in the post were changed between X2 and X3 I believe. I thought the post was a little older which is why I asked how old the post was.

 

Not sure if this has been covered yet but in your control definition are you sure you have the feedrates set to output Inverse Feed?

It is definitely set to output inverse.

this is from an mpgen 5X post..

but I'm sure your post has something similar, hopefully

where you can see it.. and not buried in the binary file.

 

maxfeedpm : 500 #Limit for feed in inch/min

maxfeedpm_m : 10000 #Limit for feed in mm/min

maxfrinv : 999.99 #Limit for feed inverse time

fix_fr : 1 #If feedrate is zero, apply these values

deffeedpm : 1. #Default for zero feed in inch/min

deffeedpm_m : 25. #Default for zero feed in mm/min

deffrinv : 9999 #Default for zero feed inverse time

 

I don't have any of this. It must be in the psb file.

 

Greg

[GPC_CNC]

Turns out that the machine control can accept F99999. I had the post edited to output on every line and now all is well.

 

Thanks for the help guys

 

Greg