[joeavaerage]

Hi,
the trajectory planner is the CNC software, that in my case Mach4, lives on the PC. It digests Gcode and then plans the trajectory by a series of discrete points at 1millisecond intervals.
The motion controller accepts that numeric data, and then generates the pulses necessary for the servos to match the trajectory.

Let say at this particular moment the X axis is at position 12345678 (a 32-bit integer) and the next time slice the X axis position is supposed to be 12345699, then the motion control knows that the
X axis needs to advance 12345699-123345678=21 steps. Over a 1ms period that means a pulse frequency of 21/0.001 or21kHz. Note the motion controller does not know or need to know the acceleration, that is what the
trajectory planner does. The PC has a lot more mathematical power than the motion controller, and it can balance the multiple acceleration profiles of the different axes involved in a move.
The motion controller can assume that the trajectory presented to it is not beyond the bounds of what the servo is capable of. That is why we take the effort to inform the CNC software of the actual
servo performance.

Sorry to say but I think your controller, being a combination of a PC and a motion controller is junk. Do yourself a favor and get either Mach4, UCCNC, LinuxCNC or Centroid Acorn.
You have spent a lot of money to get what looks to be a very useful machine but then get a sh****t controller....just to save a few bucks????. The computer part of CNC is the easy part and
a fraction of the cost of the machine hardware.

Craig

[GeckoSub]

Hi,

Sorry to say but I think your controller, being a combination of a PC and a motion controller is junk. Do yourself a favor and get either Mach4, UCCNC, LinuxCNC or Centroid Acorn.
You have spent a lot of money to get what looks to be a very useful machine but then get a sh****t controller....just to save a few bucks????. The computer part of CNC is the easy part and
a fraction of the cost of the machine hardware.

Craig

Could be the controller is junk. Though I have seen it used in a few retrofits of old machines in what looks to be real machine shops. Doesn't prove much of course.
Anyhow, I pretty much consider the controller sort of free as the machine came with it and the overall price was still well under a thousand bucks. For now, it's just a stop gap until I can get the Mesa controller board for Linux sorted and shipped/brought here. So, another 1-2 months on that. Still, of course, I would love to get the Chinese controller to work so I can start using the machine more in anger.

But I actually just thought of a way to test this out. I still somehow think it's because the servo on the Y and the stepper on the X doesn't "play well" together. Might be that the tuning on the servo is still **** and that it doesn't hit its commanded targets or something to do with me not yet having managed to kill off any remaining "smart" S-curve and smoothing filters in the servo drive.
Either way to test this, I can take the stepper from the Z and put on the Y (and move the servo from the Y to the Z). Then I will have steppers on both X and Y and if I can cut round all of a sudden, then it's not the controller. Slightly embarrasing I didn't think of testing it this way before, haha. It shouldn't take too long to move those bits around and adjust the servo gearing to match the difference in ballscrew pitches.

Maybe I'll go to the workshop now to do it otherwise, it'll be tomorrow. I'll report back.

Thanks for the spark!

[GeckoSub]

[...]
Either way to test this, I can take the stepper from the Z and put on the Y (and move the servo from the Y to the Z). Then I will have steppers on both X and Y and if I can cut round all of a sudden, then it's not the controller. Slightly embarrasing I didn't think of testing it this way before, haha. It shouldn't take too long to move those bits around and adjust the servo gearing to match the difference in ballscrew pitches.

Talking out of my butt again here. Once I have swapped the motors around, I don't need to adjust any ballscrew pitch anywhere - the ballscrews are staying put and the motors PPR don't change, either. I just need to swap the cables over in the control box between the drivers.
I think that will be today's project

[GeckoSub]

Hi,

As an experiment try on your machine deliberately setting the acceleration of one axis much slower, say one tenth of normal. Then do a G1 X100Y100 F2000 move, ie a 45 degree cut.
If your machine can do this, and I assume it can because otherwise its plain junk, then it proves that the trajectory is planned with the known accelerations.

Craig

I can't;(.
The accel setting is global for all axes. I looked under the individual axis settings tabs and no accel settings there. Only in the general tab.

[joeavaerage]

Hi,

The accel setting is global for all axes. I looked under the individual axis settings tabs and no accel settings there. Only in the general tab.

I don't believe you. I cant think of ANY credible CNC software solution that you cannot change the acceleration of each axis to match reality.

Look at the screenshot you posted, is there not multiple acceleration settings, and would not that suggest that they are for different axes?

Craig

- - - Updated - - -

Hi,

The accel setting is global for all axes. I looked under the individual axis settings tabs and no accel settings there. Only in the general tab.

I don't believe you. I cant think of ANY credible CNC software solution that you cannot change the acceleration of each axis to match reality.

Look at the screenshot you posted, is there not multiple acceleration settings, and would not that suggest that they are for different axes?

Craig

[GeckoSub]

Hi,



I don't believe you. I cant think of ANY credible CNC software solution that you cannot change the acceleration of each axis to match reality.

Look at the screenshot you posted, is there not multiple acceleration settings, and would not that suggest that they are for different axes?

Craig

- - - Updated - - -

Hi,



I don't believe you. I cant think of ANY credible CNC software solution that you cannot change the acceleration of each axis to match reality.

Look at the screenshot you posted, is there not multiple acceleration settings, and would not that suggest that they are for different axes?

Craig

Well, there are different accel settings as you noticed but they clearly state that they are for either "rapid", "feed" or that mysterious "EMC". Which doesn't necessarily prove that there should also be some for individual axes...;-)
I don't doubt however, that better controllers have this. And I will definitely have another look for more settings which I may or may not have missed.
Will also report back on this.

OK, off to the workshop, then

[peteeng]

Hi Gecko - I use UCCNC with a UC100 motion controller. So I'll discuss that but most control systems are the same. The machine controller (UCCNC or M3 or M4 or any other machine controller spits out a stream of gcode. That code only has target or max feed velocities in it. The machine controller (MC) is only interested in position not velocities, accels or jerk. The MC accepts the gcode from the CAM system "as is" initially and this will be the code you see on your screen (But its not necessarily the co-ords executed) The CAM system produces Gcode purely from geometry with no consideration of motion. The MC then analyses those co-ordinates and modifies them using its configuration rules. In UCCNC there is a linear error max, linear addition length max, corner error max and arc radius tolerance. I'm sure others have the same otherwise code could get very complex... Also note that most people run their MC in "constant velocity mode" which means the MC will try to maintain constant velocity vs exact co-ordinate contact. So the MC then pushes the modified Gcode thru to the motion controller (in my case the UC100). The code is point to point, even the arcs are descretised to a series of small lines. Since we know the velocity (and change in vel) point to point the motion controller can calculate the accel and jerk point to point while looking ahead. If the V or J values exceed the set values the V is clipped to max or less, depends on the situation and algorithm.

When you tune the axes you are determining the max accels that the motor can achieve against the inertia of the axis or any applied loads. Like driving a car you can put the foot to the floor but the car won't achieve 4g just because you want it to. Some people describe this as the reflected inertia, the car or axis can only accel at the max rate it physically can (given the motors available torque and its inertia and the axes inertia). When axes act in combination various values can be troublesome like centripetal accels around rads and if the system is not calculating centripetal accels then the machine can get overloaded. Thats why most manuals say figure out the max an axis can accel then cut it back some. So when they act in combination it has some capacity to cope with the extra loads.

So the vel, accel and in some cases jerk is calculated for each axis and if one of them exceed the set values the feed speed is clipped. So yes if one axis exceeds then the whole feed is slowed. An accelerating axis may get to its max set speed first then it gets clipped at that speed. Now constant speed means zero accel so now its travelling at constant speed. An accelerating axis may get to its max set accel before its max set speed at which point the speed is clipped at that speed and now its speed is constant accel is zero.

Some advanced systems run the gcode forward to establish an actual path vs the gcoded path, then they run that path backwards to establish another optimised path, then they run it again fwd to optimise it again (plus more adaptions as needed). This is adaptive programming. This is what a race car driver does around a track but they do fwd laps only. Each time they will brake later, change line etc etc until they feel they are getting around fastest. Now this is for roughing and air time. The final cut needs to be exact and that is usually achieved by running slow so the coded path is accurate. In some systems like robots that I used to program we had course settings and fine settings so the robot could move really fast but not accurate, but so what, then use fine settings when it had to stop and pick something up.

So to summarise - The gcode from the CAM system is modified according to the rules in the MC configuration. This new code is passed to the motion controller which figures out velocities, accels and jerk from the point to point positions in that co-ordinate stream some 300 points or more ahead say. If an axis exceeds its set max vel, its clipped at that velocity, If it achieves the set max accel before the set max velocity the instantaneous vel at that point is kept.

The MC or the motion controller does not command accels or jerk, the motor is just full bore until the set limits are hit. The limits are set by tuning the motors so they operate smoothly against their inertial or applied loads as needed. If the system has jerk control then that's another level of calculation and instead of instantaneous velocity clipping it creates a smooth velocity profile change to minimise accels... Hope that helps.. Peter

when things don't go smoothly the usual approach is to cut everything back to very slow and then slowly ramp settings up until you find the limits. But also learn about the MC tolerancing as this plays a big part in achieving smooth and accurate paths. Please note that some controllers the MC and the motion control is in the same box and are not separate. Separate motion control is a historical outcome in the marketplace when Mach3 could not fiddle with Windows clocks anymore so external clocks and calcs had to be done. This opened the commercial opportunity for separate motion controllers. My research over the last 2 years has lead me to recommend Dynomotion controllers. Excellent motion control & support in one box at a good price. Dynomotion has a forum here, worth a look. I'm about to use it on my current build router and my 5 axis router...

[joeavaerage]

Hi peeteng,

The machine controller (UCCNC or M3 or M4 or any other machine controller spits out a stream of gcode.

WRONG. The CNC software, be it Mach3, Mach4 or UCCNC accepts Gcode from a file written by a CAM program, or written by hand or manual Gcode.
The output of the software is a stream of numeric data, 32 bit integers, with each integer representing the desired position of an axis at a given time,
each block of data (multiple 32 bit integer words) representing the machine position in 1 millisecond time slices.

The MC or the motion controller does not command accels or jerk, the motor is just full bore until the set limits are hit.

WRONG. Imagine two axes that have very different acceleration but the same max speed. If a combined move is called, say a 45 degree move, ie equal distance in X and Y.
Lets assume the X axis accelerates twice as fast as the Y axis. The trajectory planner plots moves or positions along that line that both axes can match. That is to say the despite the X axis being able
to accelerate faster, it does not do so, in fact it will accelerate at the same rate as the Y axis, given that to stay on the desired path both axes must move equal distance. The trajectory planner has in effect
set the acceleration rate of the X axis to one half of its capability. Thats what a trajectory planner does.

The trajectory will allow the slowest accelerating axis to accelerate at its max rate and maintain the required toolpath while the faster accelerating axes will be accelerated at part of
their potential such as to maintain the toolpath. This has to be the case otherwise all axes would have to have the same acceleration......and that would work for toolpaths of 45 degrees,
but what about a 60 degree toolpath? Even if the axes had the same acceleration potential, one at least needs to be throttled back a bit in order to move in a straight line.

Mach3, Mach4 and UCCNC work the same way. This is evidenced by the fact that you can use a UCnnn motion control board, with an appropriate plugin, with Mach. Thus, the same basic idea
is used by both manufacturers. The trajectory planner (Mach3, Mach4 or UCCNC) plans the trajectory which perforce accommodates accelerations which the motion control board converts into pulse streams.
Dynamotion motion control boards have a Mach3 plugin and have had so for many years. Thus the Mach3 trajectory planner spits out numeric PVT (Position/Velocity over Time) data that the Dynamotion control
board can use to generate pulse streams.

Craig

[peteeng]

Hi Craig - sorry yes the MC does put out numerical data, but I kept it simple. The rest I stand by. I did say what you are saying about axes keeping in step just a different way of saying it. Of course one axis can't race away, its trying to keep the path at constant velocity or a steady accel and yes this is done by multi axis pulse streams that are kept in synchronization. The accels (and jerk if the MC has jerk control) is not set by the MC or the planner. These are calculated and clipped at the max. settings. You say "in effect" but that is a poor interpretation of what is going on... There is no executable control over accels (except by clipping it) only velocity.

Its too big and too complex to discuss motion control in this manner, better to refer to the manuals, they do explain what is going on. Peter

[GeckoSub]

A bit of an update after a few hours in the shop.
I didn't get to swap the Y servo for a stepper which would have allowed me to run steppers on both X and Y and hopefully see if that would change things.

But I did check the controller carefully and there really is just the global accel settings. Nothing on the individual axes. If someone still doesn't believe that, I can forward +30 pics of the controller tabs, but I have looked and looked and it's just not there.

I checked the backlash, too. It's not measureable. Meaning, the smallest increment I seem to be able to move the machine is 0.005mm and when I move back and forth between 0.000 and 0.005mm the dial indicator moves, too. So, whatever the backlash is, it's too small to explain this size of out of round error.

I set the accel in the controller to 20000mm/min2, it was 10000 before and much higher when the machine arrived. The 20K is a bit of a random number but it's a tad less than what the smallest Tormach machines use, so I felt maybe that could be a good start. That didn't change anything at all in the test cuts. It's twice what I had before but I have also tried faster and even slower accels. The ovality is the same.
I should also mention that the controller is a 200kHz one and that the steppers and servo are fed 1600ppr. So, we should be very, very far from overloading the controller.

I have however identified two things which help reduce the ovality. Lowering the feed rate "a lot" and killing off "smoothing settings" in the servo drive. I had already gotten a bit better results with feed rates down around 600-700mm/min. But my rough cuts are often around 2000-30000mm/min and I would think the machine should still be fairly accurate at those speeds (?). Anyways, slowing down the cuts to ~30% on the controller (so, ~200-250mm/min for the finish cuts) helped even more.

I did locate a few more smoothing and filtering settings in the servo drive and reduced and finally disabled them which improved things though not as much as slowing the machine way down. I still think this points to the servo settings being, at least, partly to blame.


I have run quite a few test cuts over the past days but the main results are these:

#1: 0.159mm error. Feed rate: 2000mm/min, finish: 700mm/min. Auto tuned servo on Y + stepper on X
#2: 0.036mm error. Same programmed feed rates as above but controller overide to only 30% on the finish so very, very slow but huge reduction in ovality.
#3: 0.146mm error. Same programmed feed rates as above, no slowing down on the controller. But changed all accels in the controller to 20000mm/min2. Not much difference from #1.
#4: 0.087mm error. Same programmed feed rates as above, no slowing down on the controller. Found some smoothing filters on the servo drive and reduced them. Nice reduction in ovality.
#5: 0.070mm error. Same programmed feed rates as above, no slowing down on the controller. Disabled the smoothing filters from test #4 fully. Even more reduction in ovality.

So, the missing test is the new servo drive settings plus slowing the cuts way down but... I really don't want to be forced to cut this slowly (~200-250mm/s). I will probably still do that test.

But the test I really need to do is to run steppers on both X and Y. I just need to machine a simple adapter plate to make that happen. Will do that tomorrow or Monday.

The first tests were done on bigger blanks and just measured with calipers. Still, even with Chinese calipers it was clear to see that something was off:


But since we are getting closer, I now cut the smaller test piece on the bottom right and use a micrometer. The features are big enough that I am certain the relative measurements are useable and certainly way better than the calipers:


P.S.
The settings I disabled in the servo drive is P1.36, P1.68 & P1.77. All set to 0 which I think disables them fully.

[joeavaerage]

Hi peteeng,
the closest I can find to a published blow by blow explanation of how it works is this:

The attached screen shot is of a Mach4 installation, nominally four axis, but with only X,Y and Z axes enabled. This is the simulator motion control diagnostics page. I was meant as a means for potential Mach4 users
to experiment, and find out about Mach4. It does not actually output any pulses as a true motion control board does, but gives the same idea.

Note how each line of output, each at 1ms time intervals have a motion command 'EX_CONT_JOG', which is presumably numerically coded to the motion control board and a block of four 32-bit integers.
Note also that the numeric value corresponds exactly to the DRO's. This does not occur in a real installation, the DRO's are a numerically processed display of the periodic return block from the motion board.
In the case of my ESS, it returns a data frame to Mach4 every 25ms. Included in that data frame are 32-bit integer positions of each axis, and presumably another 32-bit integer encoding the digital inputs to the ESS.
The integer positions describe the machine coordinate in machine steps, whatever they happen to be. The DRO is a numerically processed copy of that integer by applying the step per unit value, the work offsets, and any other
offsets in force.

Any given line or time slice is the commanded position of the machine in machine coordinates. It is presumed that the motion control board and servos do as is commanded. The commands themselves can only ever
over-master the servos if the commanded moves require higher acceleration and/or velocity that the servo can produce. Given that Mach4 is user programmed to ensure the trajectory planner knows the limitations
of each axis, it is presumed that the trajectory planner will never produce a trajectory that an axis cannot match.

Quite elegant, and yet quite simple.

If there is any real complexity or smarts it is in the trajectory planner.

Numerically it works somehat like this:

the controlled point at any given instant is x_t,y_t,z_t

There is a matrix of second order differential equations:

x_t=A_xd²x/dt +V_xdx/dt + x_t-1
y_t=A_yd²y/dt +V_ydy/dt + y_t-1
z_t=A_zd²z/dt +V_zdz/dt + z_t-1

where A_x and V_x are the acceleration and velocity of the x axis and must at all times be less than A_{x_max} and V_{x_max}, the user programmed max acceleration and velocity of that axis.
A_y, V_y,A_z and V_z are similarly described and bounded.

Note this is a second order planner, as is used by Mach3, Mach4 and UCCNC. If you wish to cause limitation of the rate of change of acceleration, then you would introduce a third order differential:

x_t=A'_xd³x/dt³ + A_xd²x/dt +V_tdx/dt + x_t-1
with the other axes following the same rationale. The coefficient A' is the rate of change of acceleration, or jerk, and is bounded by a third order planner.

The solution is thereafter matrix mathematics for which PCs are very good at.

Craig

[GeckoSub]

What I Wish I Had Known - Part 1
While the ovality issue is still the most important for me to solve - so please keep advice and ideas coming - I also learned some basic lessons already just from cutting these test coupons. I mean basic because you guys all know this but I am just putting it out there in case other beginners read this

Crashes = Blessings...
Yihaa, crashed twice! Snapped one 8mm and one 6mm end mill. No harm done to the machine and encouragingly both crashes were 100% user error and identified right away. First one was a bad fixturing job so the part moved in the vice and snap. Second was a classic, too: The WCS was just set wrong. I have set all the parts so far to have the WCS at the back left and this one, I totally forgot to set and it defaulted to the middle. Snap.
Slightly scary both times but really happy that they were explainable within seconds or minutes and that I could learn from them. Also, didn't loose much money. The alu was sourced cheaply and I am still using cheapish Chinese end mills.
I guess my point is, as long as it's not erractic machine behaviour and you figure out what you did wrong, then crashes are 100% part of the learning curve and almost a bit of a blessing - driving home some important points you have to take seriously.

Chips
Chips get everywhere and you will make more of them than you think! My machine is still a bit naked, haven't put on all the covers which I need to get done to protect the nuts and rail blocks - just waiting for some grease fittings to arrive before I button it all back up. But also, I definitely see an enclosure project in my future. I have other machines and a computer table nearby, so don't wanna spray chips all over the place. Also, I still have this naive goal of trying to keep the workshop clean

ATC...
ER collet tool changing will get really old, really fast. So far, I am using a fairly cheap 24K, 1.5KW spindle that the machine came with and so far it's not bogged down. I did shell out early on for what's supposedly one of the better Chinese 24K spindles which is meant to have more grunt low down, more poles, better bearings, etc. But it's still just ER. It wasn't cheap and I kinda already wish that I had known how useful ATC is even for the home gamer. I'd be ok with manually feeding the ATC to start with. Would just be nice not having to get the wrenches out, haha.

Coolant + Air
I need to set up MQL very soon, too. Brushing on coolant and air blasting by hand is super tedious. Fine now on the tiny parts and short machining times, but the sooner I get this done, the better. With the speeds and feeds I have been running I still managed to chip weld two 6mm polished end mills - no problem at all since I started dabbing on a bit of coolant + air.
I actually have all the parts for a peristaltic pump setup and have been experimenting with 3D printing my own nozzles and testing them at home. Not too bad, still a bit of weird cycling going on but it will work for now.

Probe
I haven't mounted my tool setter, yet, either which is a must once I start cutting real parts. Also, one of the main drivers for the switch to LinuxCNC is that I want to be able to run a 3D probe which the Chinese standalone controller can't do. A lot of the parts I will be making going forward will have 2nd or 3rd ops on them. Maybe in soft jaws, maybe not but I'd probably have to probe quite often. Again, a probe in an ATC would be sweet though.

I have probably read all this advice in snippets here and there before. But it's like that I would still not have shelled out for a lot of these things thinking I am just a beginner and these are more pro features. But if you plan on cutting just a bit more than the odd one-off and you're trying to keep a somewhat clean space, I'd say they are really worth considering from the get go.

OK, back to the ovality issue. Next up I'll move the Z stepper to the X and have steppers on both X and Y. I am hoping that will cure the problem which should mean that it is the servo tuning/settings that are off. And it will buy me some time as I can start making some better, real parts until I figure out what to do next.

[peteeng]

Hi Gecko - I interpret your symptoms as a tolerance issue not a motion control issue. So a) investigate the tolerance settings in your CAM program and b) investigate the tolerance settings in the machine controller/motion planner.

Hi Craig - by the time the executable info is at the motion planner its a stream of pulses. It can't be differentiated as it's not a continuous function, its a contiguous stream of pulses. Each pulse is a step or a microstep. So we know the distance of each pulse, the timing of the pulses give it velocity. So now we know the distance and time, start and end velocities point to point the accel can be calculated simple with V=U+at. or V2=U2+2as... no differentiation need. I also saw the comment about rapids and feeds being different tolerances. At each step of the way the controller knows if its in material or in air via the Z ht. At some point we have told the system the top ht and bottom ht. So there will be a logic (is the z<top>bottom?) if yes, its a feed, so use feed tolerances. If Z>top then use rapid tolerances... I'm sure this is a tolerance issue. Peter

[GeckoSub]

Hi Gecko - I interpret your symptoms as a tolerance issue not a motion control issue. So a) investigate the tolerance settings in your CAM program and b) investigate the tolerance settings in the machine controller/motion planner.

Peter

Hi Peter,
The CAM is Fusion and while the tolerances aren't tight for the adaptive strategies at 0.1mm, I have made sure to set more radial stock to leave than the error. I have 2D Contouring as a finishing strategy with a tolerance of 0.01mm so still 4-8 times smaller than the error. It's taking small stepovers and I also have spring passes on these features all at a slower feed rate and none of the finishing passes even touch the floor, only the sides (I am getting really decent side wall finishes to my untrained eyes, so that's at least nice, haha). In practical terms, I am doing what I can to make sure no deflection or other weirdness is happening on those final cuts. I can also hear that the finishing strategy does cut on all sides so it's not like the adaptive has already cut too much.

The controller has a 'Contour Accuracy' which is the only thing that sounds like a tolerance setting in it and I've run the last few tests at 0.005mm - down from 0.020mm in the earlier tests.

I can try dropping the tolerance even more but I think 0.01mm is already pretty tight?

Anyhow, that part only takes a few mins to cut, so why not

[EDIT]
This message never got sent, but that's alright as I cut the test now and can include the result:


Tolerances for this test were lowered to 0.001mm in both Fusion and the controller.
Error is now 0.066mm down from 0.070mm in the previous test which is an ~6% improvement but as I changed a few other serttings ever so slightly - added one more finishing pass - we can call it even. Yes, I know I should only change one parameter at a time, my bad.

Anyhow, I don't think that lowering the tolerances were a miracle cure.

I speculate that it's the servo over shooting its position because of less than stellar tuning - which I would assume gets worse as the speed increases. I tried to get the scope to work in the servo drive yesterday but still roaming around a bit blind but I think I saw some follower errorw in the range of 50-85 pulses. But I don't know if those are encoder pulses and whether its native pulses or the reduced ones I have set or the PPR pulses I have set in the controller. Most likely one of the two first, though.

However, these tolerances are definitely good enough to cut the riser plate I need to make the servo-stepper swap work. So, lunch now, and then cutting the riser plate.

[peteeng]

Hi Gecko - I have been using Fusion CAM for about 1.5 years. I have found that the "tolerance" setting in 2D contour does make a difference so I run it at 0.001mm. There is also a smoothing tolerance if you use smoothing. There is also a tolerance in the post processor, did you know about that one? See attached. Maybe make the minimum chord length smaller...
My main concern would be the linearisation strategy and arc tolerance settings in your machine controller and/or the trajectory planner. I did some tests with a simple circle in Fusion using different tolerance settings and the resulting gcode was always the same. It discretised the circle into 4 arcs which is typical. I expect things like splines would get more interesting.. Smoothing turns spines into a series of tangent continuous arcs within the tolerance. Not sure I like that, but it does make for more efficient coding. For instance I make aerofoils and hydrofoils occasionally and I'd prefer the surfaces / curves to not have curvature discontinuities in them so I wouldn't use smoothing in that instance.. Peter

Just a thought - In creating a circle the XY motors/drives has to stop and change direction twice every 360deg. Does the egg shape agree with the axis directions? If so this may point at a mechanical hysteresis issue

[GeckoSub]

Hi Gecko - I have been using Fusion CAM for about 1.5 years. I have found that the "tolerance" setting in 2D contour does make a difference so I run it at 0.001mm. There is also a smoothing tolerance if you use smoothing. There is also a tolerance in the post processor, did you know about that one? See attached. Maybe make the minimum chord length smaller...
My main concern would be the linearisation strategy and arc tolerance settings in your machine controller and/or the trajectory planner. I did some tests with a simple circle in Fusion using different tolerance settings and the resulting gcode was always the same. It discretised the circle into 4 arcs which is typical. I expect things like splines would get more interesting.. Smoothing turns spines into a series of tangent continuous arcs within the tolerance. Not sure I like that, but it does make for more efficient coding. For instance I make aerofoils and hydrofoils occasionally and I'd prefer the surfaces / curves to not have curvature discontinuities in them so I wouldn't use smoothing in that instance.. Peter

Just a thought - In creating a circle the XY motors/drives has to stop and change direction twice every 360deg. Does the egg shape agree with the axis directions? If so this may point at a mechanical hysteresis issue

Hi Peter,
Thanks for these pointers. Though in the meantime, the swap to steppers looked to have solved the issue and I am down to about 5um of ovality. Have to run a few more tests to confirm this but it's looking promising. (See my previous post above).

I didn't know there was a tolerance setting in the post processor, too. I just had a look and it's at 0.002mm so that's alright. Minimum chord length is 0.25mm and Min. circular radius is 0.01mm like yours.

I have turned smoothing off in Fusion for these tests. But I also see a lot of G03s in the code so I think the round boss is being cut with "proper" circular commands and as such, I don't think smoothing would have had an impact anyways? I think it's only for splines as you say.

Anyhow, I will probably adopt your settings overall.

Also, the ovality was always at the same "angle" always at 45d.

I am left with this weird glass half full/half empty take on this, though. On one hand I am super stoked that it looks like I can cut this accurate and I can start cutting real parts. But it bums me out not being able to make the servo work. I have four of these servos sitting around and I really want to make them work.
I have read horror stories of tuning issues before but have also read about people running auto tune and gotten their servos to run flawlessly with just that. But yeah, it seems I have to do the hand calcs as Craig suggests so that will be for the second go at this - once the remainding servo motor mounts turn up. And then learn to set up and use the built-in scope properly to diagnose follower errors.

Before I battle the servos again I have to get the machine trammed even better. There's a granite precision square on the way by now so that will be fun/frustrating, too

P.S.
Interesting on your airfoil/hydrofoil work, btw! I used to race sailboats back home and dreamt of being a naval architecht so did look into foil design for a bit many moons ago. And actually, I may build a little RC sailboat here and knowing myself I will want good foils on it, so even though it's overkill I might cut an alu mold for the fin and rudder, haha

[GeckoSub]

It's Not The Controller...
I got the riser plate made so I could swap the stepper on the Z for the servo on the Y. So, now I have steppers on both X and Y and the results are in.
Same file, same g-code, only got rid of the servo. The stepper-only test is #7 on the right:



The error is down to 0.005mm on the 11mm boss. Which is "perfect". Strangely enough, it's 3 times higher on the square at 0.015mm. But it's getting late now, I am knackered and it wont be smart to cut more tonite.

So, if the steppers can cut round and I can't when I mix one stepper and one servo, I think the conclusion will have to be that it's something to do with the servo. As mentioned, I think the tune is off and it's overshooting its marks or something like that. Had a random idea but probably it's bullocks but I wonder if the servo really doesn't like being only fed 1600PPR. I did that to simply things and keep it the same as for the steppers. As I said, it's prolly nothing.

Anyways, this is "good", kinda, I guess... haha.

As for the riser plate it's the first functional part I have cut on the machine and it came out nice enough for my first real part. I had some cast, ground plate in 6mm thickness but had to deck it down to 5mm which worked pretty well. I think it's 0.025mm or so off in one corner. Then I bored eight holes - really slow to make sure they were round enough. Hand tapped four of them, the others are clearance holes. But the latter needed a big chamfer for some countersunk screws so I did that with a 3mm ball nose endmill and a lot of fine stepping down. Worked super well.
Some (deep) witness marks from me still touching the tools off on the part itself. But for this part which is now hidden under a motor mount, I don't care


I still really need to get the servo issue solved. Yesterday, I ordered the two remaining servo motor mounts so I can run them on all axes. The mounts will here in about a month but I wanted to start cutting some parts so that's why I ended up trying steppers only on the X/Y. This buys me a bit of time, but I sense some headache in the future on this matter...

[joeavaerage]

Hi peteeng,

can be calculated simple with V=U+at. or V2=U2+2as... no differentiation need.

Numerically there is no differentiation, but is set up as a multi-order difference table.

In the case of a second order planner the difference is two orders 'deep', ie equivalent to d²x/dt². With a third order planner the difference table is extended to
three orders deep, the equivalent of d³x/dt³.

The idea is very similar to a matrix State-Variable problem beloved of Systems and Control Engineers. Despite looking like a first order system, ie one differentiation (analytically) or difference (numerically),
if an output (differentiated) is also an input to the matrix, it is in effect differentiated a second time, and in similar manner it that output is listed as another input then it is
differentiated a third time. Thus with what appears to be a first order matrix can in fact describe a multiple order differential equation.

The beauty of this State-Variable formulation is that it can be automated. You supply the coefficients of the matrix to represent the mathematical model of the system and a computer will automatically solve for
the matrix Eigen function, which is the equation of motion of the complete system. I spent three tough years at University studying this stuff, any Electrical Engineer had to do so, it was not optional and represented
about one third of the core course work with communication theory and electromagnetic theory being the other two thirds. Mere computers, or electronics, or power systems were all optional, you chose what you
thought you wanted to do after graduating, but everyone had to pass these core subjects....and they are not for the feint hearted!

Craig

[GeckoSub]

Fixture Plate #1 - How Many Holes...?
I plan on making a fixure plate as one of the first bigger projects and I need to start ordering materials and hardware and settle on the design.
The idea is to buy cast, ground alu tooling plate. Hopefully cut fairly precise and then I'll mill and tap all the bores myself. The thickness I got in this material last time was impressively consistent.

While I do want it as big as I can get it, I am being very careful to make sure I can actually reach where I need to with the travels I have. I have two insert end mills in 20/35mm incoming and I think I can run at least the smaller one for facing. So, the max travel + plus the diameter of the "face mill" minus a wee bit will decide the size of the plate. Yep, I am willing to give up on being able to mill the sides/outline just to make it a tad bigger. But I will be triple checking all this before I order the plate.

It will have a pattern of bolt holes (of course) but the first question is, how many bolt-down holes to secure the fixture plate to the T-slot table would you think is sufficient?
The fixture plate in this revision is 380x430mm. I have four T-slot channels in the table and right now, I have it modeled with three screws in each so 12 in total. Which must be overkill?



Also, on a related note, this CAD will soon have the underside features so I can ask Fusion to give me the total weight of it all for the inertia calculations for the servo tuning

[joeavaerage]

Hi,

how many bolt-down holes to secure the fixture plate to the T-slot table would you think is sufficient?

Why??? The Tee Slot table is designed and built with the idea that you can clamp workpieces direct to it via toe clamps or mount vices, jigs or anything else.
Why bother making an expensive fixture plate to sit on top of it? If the fixture plate were sacrificial, like MDF or a thick acrylic then maybe. I make a lot of small parts using that method.
I have a fixture plate of 10mm acrylic that I can hold in the vice, the vice being held down to the tee slot table with bolts/tee nuts. The material is clamped or often stuck down with double sided
tape to the acrylic. I am not at all concerned when the tool passes right through the material into the acrylic underneath as it is sacrificial. I flip it over when the top side is that scarified that double sided
tape no longer sticks to it. Using both sides I replace it monthly roughly.

I started doing this because I make a lot of circuit boards with my machine, but the technique is applicable to other jobs and materials.

The joy is that you can easily remove it from the vice, one or two seconds, load or re-load the fixture with material then put it straight back in. There is a stop on the mounting section of the fixture plate that allows me to
put in back in in exact position as it came out....saves having to re-touch-off all the time.

CNC is often about finding a simple, cheap and repeatable, with emphasis on repeatable, procedure or fixture.

Craig