Siemens 4th axis, wrapped toolpath, erratic feed rates issue

[workshopB26JU]

Hey I'm hoping this is a relatively straight forward post/programming issue.

we have a basic right hand, 4th axis  around X set up on a 3 axis VMC 

the control is a Siemens 828 using a modified 840 post 

we are getting A axis code so no cycle 800, or Traori issues.. which is good 

So far we’ve tested the post using 4th axis for indexing moves which work absolutely fine.  A 0.00  A90.00 etc etc…

What I’m trying to do now  is wrap a slot 8mm wide 4mm deep  around a 50mm dia bar.

So I cam’d it up, using a sample post processor  benchmark model within Fusion and ran the program ..

The tool path itself looks fine, the problem is with the 4th axis motion feed rates!!!

The federate in the program is set to 100mm/min "see photo of cutting data"

The tool feeds in to depth “1mm D.O.C” radially @100mm/min,

then machine feed rate switches from mm/min  to degrees per min ??

 “which my 5mm tool can handle”  the 4th axis continues to rotate to A340

The tool then rolls around the rad in the X axis  then the 4thaxis rotates back to A 188 angle much faster than it did when rotating @ deg/min this is while the tool is still engaged..   “basically to fast for the tool to handle with the machines over ride set at 100%"

See sample of program below N195 – N219

So my question is:

Looking at the sample of the program below there is just one F100 feedrate @ N27

Although when the program is running there appears to be several feedrates while the tool is engaged?

A combination of deg/min and mm/min ??

should there be more F values ?? 

would you expect to have an “F” feed value after the Z & A value on each line?

Once I know how the program should look and run safely I can find where the missing link is…

Initially I was thinking is the issue with the 4th axis set up or parameter settings ?

Now I suspect maybe a motion setting in the post.?

I just need a starting off point to know where to go next.  

any help would be much appreciated

Thanks 

Martin

 N22 G54

N23 G0 A273.133

N24 G0 X70.3 Y0 Z40

N25 M8

N26 G0 Z30

N27 G1 Z28 F100

N28 S5000

N29 G1 Z27.755 A272.958      N27 Should there be an F value for each move?           Also it looks like the A moves increment at about 2/3 degrees at a time ? does seam about right?

N30 G1 Z27.573 A272.478

N31 G1 Z27.5 A271.816

N32 G1 Z27.467 A269.204

N33 G1 Z27.433 A266.591

N34 G1 Z27.4 A263.979

N35 G1 Z27.366 A261.366

N36 G1 Z27.333 A258.754

N37 G1 Z27.299 A256.141

N38 G1 Z27.266 A253.529

N39 G1 Z27.232 A250.916

N40 G1 Z27.199 A248.303

N41 G1 Z27.166 A245.691

N42 G1 Z27.132 A243.078

N43 G1 Z27.099 A240.466

N44 G1 Z27.065 A237.853

N45 G1 Z27.032 A235.241

N46 G1 Z26.998 A232.628

N47 G1 Z26.965 A230.016

N48 G1 Z26.932 A227.403

N49 G1 Z26.898 A224.791

N50 G1 Z26.865 A222.178

N51 G1 Z26.831 A219.565

N52 G1 Z26.798 A216.953

N53 G1 Z26.764 A214.34

N195 G1 X70.295 A351.764

N196 G1 X70.296 Z24.11 A349.075

N197 G1 X70.298 Z24.076 A346.386

N198 G1 X70.299 Z24.041 A343.698

N199 G1 X70.3 Z24.007 A341.009

N200 G1 Z24 A340.467

N201 S7958 -------   this is where the feed rate shoots up from A340.467   to    A188.215 but there is no actual change in F value ??

N202 G1 A188.215

N203 G1 X70.29 A188.184

N204 G1 X70.275 A188.141

N205 G1 X70.25 A188.081

N206 G1 X70.217 A188.011

N207 G1 X70.175 A187.933

N208 G1 X70.125 A187.853

N209 G1 X70.069 A187.772

N210 G1 X70.006 A187.695

N211 G1 X69.938 A187.624

N212 G1 X69.867 A187.562

N213 G1 X69.794 A187.51

N214 G1 X69.718 A187.468

N215 G1 X69.644 A187.438

N216 G1 X69.571 A187.421

N217 G1 X69.46 A187.412

N218 G1 X68.538

N219 G1 X68.422 A187.421

[Anonymous]

I see that there is a speed increase at the point where feed rate shoots high,........... soooooo what happens if you delete that speed code?,....... I would expect feed rate to stay constant as it relates to other parameters like chip load per tooth at certain speed.

[workshopB26JU]

Hi @Anonymous 

Thanks for taking the time to reply. 

I'm relatively new to Fusion so I could be wrong here...

i See what you are saying , but i thought the S always referred to the spindle speed 

& F represents the feed rates ?

see below a section of the same program.

N18 ; Wrapped pocket roughing
N19 T="EM5A" D1
N20 M6
N21 S7958 M3
N22 G54
N23 G0 A273.133
N24 G0 X70.3 Y0 Z40
N25 M8
N26 G0 Z30
N27 G1 Z28 F50 -------- the F value only appears once on the entire program .
N28 S5000       --------- where as there are several S value changes  depending if the tool is ramping or engaged ?

N29 G1 Z27.755 A272.958
N30 G1 Z27.573 A272.478
N31 G1 Z27.5 A271.816
N32 G1 Z27.467 A269.204
N33 G1 Z27.433 A266.591
N34 G1 Z27.4 A263.979
N35 G1 Z27.366 A261.366

Thanks 

Martin

[GeorgeRoberts]

Good morning,

It looks like the problem is that the post processor you're using is outputting feed per min rather than degrees per min. Can you share a copy of the post? 

[workshopB26JU]

HI @GeorgeRoberts 

Thanks for your time.

again I can see what your saying, up until now we've only used the 4th axis for indexing moves so guess the feed settings in the post wouldn't have been an issue ??

I've attached the post we are using.

the post itself is a modified 840 post with the B & C section removed so should just read the A values .

probably not relevant but I've set the direction for the 4th axis to positive 

"rather than negative, or don't mind" like I say 

don't think this should matter but thought I'd mention it any way.

Thanks Martin 

[Anonymous]

Well, program shows feed per minute and value is related to spindle speed and chip load per tooth, so my suggestion was to delete that increased speed and see what happens.

My expectation would be that feed rate would remain constant based on the fact that initial feed rate was calculated in relation to spindle speed at the top of the operation and only obvious factor for its change would be increased spindle speed at turn of the tool path.

Now, I am not familiar with Siemens control so I am not sure if occurrence of higher spindle speed at turn of tool path would result in adjustment to feed rate without actually displaying higher feed rate in program.

Whether inches per minute or degrees per minute are correct format for your machine, spindle speed plays role in calculating its value.

Have you tried deleting that second spindle speed and if so, did it make a difference?

[workshopB26JU]

Hi @Anonymous 

sorry I should have ended my last message to you by saying I will definitely try your suggestion.

I've edited the program, and as soon as the machine is free "which will be early tomorrow morning" I will test your theory and let you know the results..

If that is the case I'm assuming the post can be altered to stop the unnecessary S values appearing in the posted program. ?

Thanks 

Martin 

[workshopB26JU]

Hi @Anonymous 

Firstly I did as you suggested and removed the S5000 values from the posted program.

"I did this on the control" 

I ran the program, unfortunately it made absolutely no difference.

while the tool is engaged in the part during the programmed geometry, the 4th axis rotates at 

degrees per min.

then during the repositioning moves/ramping moves 4th axis rotates in a rapid traverse move. which is far to aggressive for the tool ??

So now I'm trying to figure out if this is a CAM issue on my part ???

or a Post issue as @GeorgeRoberts suggests??

Just to recap we're using a 5mm tool to produce a 8mm slot using the wrapped toolpath.

I've made a screencast to show exactly what is happening in the simulation 

I do have a question though that isn't clear on the screen cast..

at line 236 the 4th axis repositions from A193 to A351

the posted program shows no change in feed rate ??

and it's not obvious in the simulation either .

but when the program is running this move is definitely an aggressive  rapid 4th move??

so is this a post issue ?? 

N232 G1 X67.735 A188.132
N233 G1 X67.718 A188.187
N234 G1 X67.705 A188.236
N235 G1 X67.704 A190.925
N236 G1 X67.702 A193.614

                                                  the 4th axis repositions at this part of the program as a rapid move.
N237 G1 X67.7 A351.785
N238 G1 X67.71 A351.816
N239 G1 X67.725 A351.859
N240 G1 X67.75 A351.919
N241 G1 X67.783 A351.989

Hopefully this makes sense?

thanks 

Martin

[GeorgeRoberts]

If your machine is expecting degrees per min and it's outputting like you show in the sample, I think it's a post issue. 

As a start, you could try changing this:

  if (true) {
    var aAxis = createAxis({coordinate:0, table:true, axis:[1, 0, 0],range:[-360,360],preference:1});
    machineConfiguration = new MachineConfiguration(aAxis);

    setMachineConfiguration(machineConfiguration);
    optimizeMachineAngles2(1);
  }

To this:

  if (true) {
    var aAxis = createAxis({coordinate:0, table:true, axis:[1, 0, 0],range:[-360,360],preference:1});
    machineConfiguration = new MachineConfiguration(aAxis);
    machineConfiguration.setMultiAxisFeedrate(FEED_DPM, 9999, DPM_STANDARD, 0.5, 0.5);
    setMachineConfiguration(machineConfiguration);
    optimizeMachineAngles2(1);
  }

 That will convert the feeds to a standard degree per min output with a maximum feed of 9999.

Before making this change, ensure you backup your existing post processor and test any output very carefully

[Anonymous]

As I sad, I am not familiar with Siemens control so I cannot speculate on possible solutions but I am trying to connect few dots.

From information you provided in your posts, I generated radial slot and posted it using your post, in attached files you can see that feed rate resulted in mm / minute, one for ramping and one for cutting which is not evident in NC code you posted so I am puzzled with that.

I don't have my backplotting software coordinated with Siemens control so I commented out few statements to be able to produce backplot of tool path.

I hope attacked files can provides some clues but otherwise I am not qualified to resolve your issue other then to say, A axis tool path wrap work may need feed type converted to degrees per minute in your post as suggested above.

[Anonymous]

Here is NC file posted for Haas and using degrees per minute, note that feed rate changes constantly because formula is considering change in diameter for every segment of tool path, hope that provides some clues for you.

[workshopB26JU]

Hi @Anonymous 

You mention being sad? 

I'm the one sat here pondering over your words on a Sunday afternoon!!!

I've tried your model to post out some code on my system to see what results I get,

like you say your version has constantly changing feed rates along side the A values, 

where as mine still only has the one  F200 at the top of the program .??

leading me to think it must be a post issue .??

I'll carry on trying like you say to join the dots on this one..

Thanks 

Martin

[workshopB26JU]

hi @GeorgeRoberts 

As you both say the signs suggest this is a post issue.

I've changed the lines you suggested.

The result when I posted the program was the program settings options didn't populate which isn't a good sign in my experience .

I continued to post the program,  the result was as expected.

the dreaded error page!!

Error: Failed to evaluate post configuration.

Code page changed to '1252  (ANSI - Latin I)'

Start time: Sunday, October 11, 2020 5:10:55 PM

###############################################################################

Error: SyntaxError: return not in function

Error at line: 381

Failed while processing global script.

###############################################################################

Error: Syntax error: Unmatched } at line 402.

line 381 below:

 if ((getNumberOfSections() > 0) && (getSection(0).workOffset == 0)) {

    for (var i = 0; i < getNumberOfSections(); ++i) {

      if (getSection(i).workOffset > 0) {

        error(localize("Using multiple work offsets is not possible if the initial work offset is 0."));

        return;

      }

402:

  writeBlock(gFormat.format(64)); // continuous-path mode

  writeBlock(gPlaneModal.format(17));

}

I'm afraid both these lines mean very little to me, 381 multiple work offsets is not possible if the initial work offset is 0 

I'm not sure what this is referring to ?

only thing that springs to mind would be in the

passes tab

sideways compensation "left, climb milling"??

as far as 402 continuous path mode ?? 

I've drawn a complete blank on that one I'm afraid.

sorry I couldn't be more helpful .

Martin 

[Anonymous]

I mentioned not being familiar with Siemens control but it seems that it requires feed in degrees per minute for A axis and you are getting feed per minute instead.

In my sample, feed changes for every segment on tool path that has diameter change, namely fillets on both ends of slot and again on second depth pass.

In recent months I had to adjust post to produce degrees per minute for C axis work on Hyundai Wia mill-turn, I stumbled into statement that did the job but I am not able to pinpoint that section of post for you because I don't know the specifics about your control.

As an alternative and to get you going, you could post your job using any post that produces degrees per minute feed output then edit top and bottom of resulting code for tool call and A axis commands required by your machine. 

[Anonymous]

It looks like I uploaded wrong NC file with my sample in earlier post so here it is again, posted for Fanuc mill with A axis.

[Anonymous]

Here is Siemens post from HSM library set to X rotary table, ..... are we getting any closer?

[workshopB26JU]

Hi @Anonymous 

Could be on to something here...?

using the generic 808 Siemens post

" no modifications made"

to post out code for the original program used in this thread and there are various feed rate changes .

not at every A axis move, but definitely more that i was getting using my original post 

"which is a modified 840 post set to read A axis in a positive direction"

if I'm honest I don't know how to tell if the feed rates are posting out as degrees per min, or mm per min ??

how can you tell this ?

sorry if it's an obvious question  ..

Thanks 

Martin

[Anonymous]

How to tell ?...... well I'll go back to day I ran repeat job originally done on Haas and second run done on Hyundai Wia mill-turn. After obvious edits to get bulk of the program adopted I was looking at C axis barely moving, way out of sink with Haas.

It's that obvious that something is not right, I was lucky to have found the right statement in post processor, took a chance on changing one statement, reposted the operation and there it was, nearly every line had drastically different feed rate from one in Haas program.

So that worked out fine and tool was cutting at seemingly same pace as I recall seeing in Haas.

I did some snooping on Google and came up with some formulas and explanation on how to calculate degrees per minute but all I cared to remember is the fact that feed rate changes in relation to diameter tool is on and I never looked back.

Also check this link:

http://theoreticalmachinist.com/4axisCalcs.aspx

Convert few feed rates to IPM and note the relationship.

Take a tool out so that coordinates are in sink with given feed rate, run program and see how it behaves, you should be able to make visual estimate of cutting pace and any changes that don't seem right.

[GeorgeRoberts]

Sorry for the delayed response, i've only just seen this! 

Looking at your first image, you have an extra '}', just delete that and the post should work again.

This will activate the DPM feeds and hopefully should run a lot smoother!