Siemans 810d post problems.

[DazE]

Hi all,


Has anybody got any ideas how to reslove a problemI am having with my post?


The problem only arises when I want to output large 3d surface machining programs. If I use the parameter setting "points only" the program will run in the machine but it will be large and results in machine judder when milling radii. If I use the parameter setting "Points and arcs" I get a much smaller program and the milling is far smoother. However when I use "Points and Arcs" I get a "circle end position is incorrect" error at the Simens810d control at some point during the machining.


I know it is something to do with a cumlaltive error generated by the post but I am not sure what settings I should be looking to alter.


Does anyone else use this control with Prismatic Milling?


Thanks


Darren

 

[indigo2]

Darren -
Couple of possible options for you.
First, make sure the arc format you are outputting is correct. Meaning that the IJK register outputs are in the right format. There are four options for Absolute, and three for Incremental. This option is found under the Motion > Circular area in the Option File Generator.

Next thing to check is under the Motion > Circular > General tab. There is an option to have the post do a minor correction to the arcs for you. It is the third option on the right, Correction Method. The post can either add a small linear move at the end, or make a correction to the arc radius.

That give you some options to test. I am sure there is a combination of those things that will work for you.

Regards-
-tsl

 

[DazE]

Hi,


Thanks for your quick reply.


I had already discovered the "Correction Method" and although it seemed help with smaller programs I still get the error on larger d surface machining.


I have not tried to alter the IJK register outputs before and so this will be something to try this afternoon. Currently they are both set to " start point to centre distance signed". Do you have any suggestions as to what would be a good alternative?


Thanks again for the help.


Darren

 

[indigo2]

Darren -
I can't really say which is the 'best' alternative.

I think it is more a question of which (of the 4) option matches what the controller is expecting to see. I guess the worst case scenario is the you have a 25% chance of getting it on the first roll.

A better method for determining the correct format would be consulting the programmer's manual for that machine, and following that format.

-tsl

 

[DazE]

Hi,


I am working through the possible combinations at the moment but so far no luck. The original settings actually seem to give a result which matches the machine code but as I said there seems to be a numerical error. I think perhaps it will be an absolute setting which would give a cumlative error rather than the incremental settings. Ill keep on tweaking until the boss notices the machine is not running

Thanks again for your help.


Darren

 

[marker4x4]

....I had already discovered the "Correction Method" and although it seemed help with smaller programs I still get the error on larger d surface machining.

Make sure that your Maximum Radius is set large enough to cover your surface's rad...
Some lofts have REALLY big rads, so your post may clip it. But on the second thought, that would result in error in your *.lst file, so make sure you check that too.

Good luck

 

[orac]

Do you know whether a G9 or a G64 is active on the Siemens control ?
If it is G9 you will have a very accurate positioning which leads when many points are involved in some kind of shaking/trembling of the machine. Try to place a G64 in the first lines of the program. Perhaps this can give better results.

Best regards,

John Bijnens

 

[DazE]

Thanks for all the suggestions.


So far I have tried every combination of the ijk register inputs. However every other combination gave a slightly worse result than my original settings...still it was worth a go.


My maximum radius setting looks good as I have no problem with large rads in small programs. Only lots of rads in big programs givesw me the error.


Our machine already has the G64 active in the first line of all our output programs but thanks for the suggestion.


I have decided to try and output the programs with 4 decimal places to try and increase the tolerance. I went into the post and noticed that under the MCD File Format my settings state "4before" and "6after" the decimal place(nnnn.nnnnnn) for each axis. However my output files are always to 3 decimal places(nnnn.nnn). Does anyone know how to set the number of decimal places that the post will output at?


Thanks again.

 

[MR_NC]

Sorry the picture is so BIG! No time to rescale.
Make sure your config.pro has the options highlighted as shown in this pic (see bottom). The picture also shows how to control .xxx output. Make note, that you will need to change this for any axis designation you are using I.E. (ABCXYZIJK,etc).

The reason the config option matters is that if Pro is "thinking" .xxx and you wish to output .xxxx that data you want to output does not exist.

I also suspect that the global tolerance is at play here. If the 810D wants arc's "right" to .xxxx then you shouldn't be using something .xxx for global tol. Guessing here more than knowing.

Also, FWIW in my experiance using post options like correct CL arc points, etc. Only results in pain...

LAST! But possibly MOST important (not real up to speed with the 810D) MAKE SURE you are not fighting something MACHINE SIDE! Many machines have a param setting for arc endpoint eval. This needs to be something reasonable. Not something .xxxxxxx unless that is the work you do...

All I got, hope it helps.
Best regards,
Sean

 

[DazE]

Mr_NC


Thanks for the pic.


I have already experimented with the Register settings in the Mcd File and regardless of what I have set (currently set to 6 dec places) my output Nc file is still only to 3 dec places. There must be another controlling factor somewhere.


I did not have those settings in my config.pro but I understand that the default is to ten decimal places. My ncl files are to 10 decimal places already. However I did add it anyway but it made no difference unfortunately.


I am currently in contact with our machine supplier regarding the chances of it being something machine side. So far however it would seem our Parameter setting for arcs is set to .001 which seems quite reasonable to me. I think perhaps if I set it to .01 the program may work but not at the accuracy I desire. This is why I am trying to output to 4 decimal places to see if that makes any difference.


Thanks for the help.


P.s Where would I find this Global Tolerance?

 

[DazE]

Hi,


Below is a small section of my program. I am pretty sure it fails herebecause of the missing J on the 6th line down. Does anyone have any ideas why my post should decide to not output the J and cause me misery? Bearing in mind that this program will run for 7 minutes before it gets to the offending line and stops my mill dead.


Any thoughts much appreciated.


Darren


G1 Y-24.915
G2 X158.007 Y-34.563 I-9.727 J0.
G1 X158.007 Y-34.563 Z-4.452
G2 X63.309 Y-43.042 I-158.007 J1231.575
X62.553 Y-43.034 I.03 J6.065
X61.93 Y-42.955 I.449
X61.114 Y-42.75 I1.079 J6.027
X60.521 Y-42.523 I1.92 J5.9G1 X63.293 Y-43.043
G2 X62.97 Y-43.05 I-.289 J5.77
X59.764 Y-42.125 I2.557 J5.775

 

[orac]

This looks like there is a coordinate optimization where the J command is probably the same as in the previous line.


Try to put this optimization off. I don't know GPOST, but I suspect it is called "optimization" or "modal/non modal" mode. If the latter then choose non model.


Best regards,


John Bijnens

 

[marker4x4]

This looks like there is a coordinate optimization where the J command is probably the same as in the previous line.

Ditto that. Try this (the two OTHER boxes on the bottom):

View attachment 3905

 

[wsylvester]

easy test would be to copy the ijto that line and see if it gets to the next

 

[dbrainsky]

DazE,


Have you tried setting the the circleoutput in the gpostto non-modal? Seteverything including the IJK. Also check to insure that the circle output is set for every 90deg instead of default quadrant crossing.


Another option in the gpost circle panel has to do with tolerance in Z before outputting G01. Since your forcing 3D circles you should expect to see IJK in the output file. With the Z tolerance setat default at .001 then G01 will be output. Set this value to 0.000000.


See pic for non-modal ijk gpost panel


Dave

 

[DazE]

HURRAH!!

Knowing that the problem was just the missing J and not some strange numerical error was the key. I unticked the "IJK code modal" box as shown in Marker4x4 picture and it seems to be working. My only worry is that my PTC support guy sent me another post to try which also works but has that option ticked! I cannot get hold of him to query this until tomorrow but for now I am just happy that the machine is running again. Last week I had no posts that worked and then just like buses I now have two that seem to work.


Thanks to everyone who tried to help

Darren