My sizes are out

[Desertboy]

Hi, I've been almost exclusively 3d carving and sign making never noticed my sizes are out.

I cut a simple hose adapter a few times now and every time it's out but exactly the same amount, tried 3 different tools to cut it, from 1/2" to 1/8" end mills.

I'm out by ~1mm on 33mm hole, the holes are round and all 4 cuts are out by the same amount, tried it fast and super slow the same.

1610 Chinese ballscrew's from alixpress, direct drive, AM882's, 70v PSU, motors barely get warm after an hour of 3d carving.

DDCSV controller generated gcode in Fusion and vcarve same results.

What can be causing it and how do I solve it?

[Neale]

Sounds like your "steps per unit" calculations have gone a bit wrong. Can you recheck, or post all relevant data here so someone else can check your working?

The other way of doing it is starting with a good first guess - which you have - and then modifying the "steps per" based on the results of a calibration run. Personally, if my calculated value were out by more than a tiny amount then I reckon something's wrong - my calculation or a machine error. Slipping coupling, missing steps, or whatever. However, others take the more empirical approach. In short - keep tweaking until you get the right answer! Mach3 actually has a calibration capability built-in but don't know about your controller.

[Desertboy]

Sounds like your "steps per unit" calculations have gone a bit wrong. Can you recheck, or post all relevant data here so someone else can check your working?

The other way of doing it is starting with a good first guess - which you have - and then modifying the "steps per" based on the results of a calibration run. Personally, if my calculated value were out by more than a tiny amount then I reckon something's wrong - my calculation or a machine error. Slipping coupling, missing steps, or whatever. However, others take the more empirical approach. In short - keep tweaking until you get the right answer! Mach3 actually has a calibration capability built-in but don't know about your controller.

On the ddscv it's steps per mm

I have 8 microsteps
so 8*200/10 (1610's) for X&Y 160
320 for Z (1605)

Just double checked this is definitely what they are set to.

AM882 has fault protection it should detect missing steps and estop and I swapped all the couplings for these style, I bought the chunkier ones.

27689

so they're rated twice the nm of the motors.

2 4nm in the bottom and 3nm on the gantry, PSU is 70v and 1kva.

Will try and cut 3 holes at 33mm, 66mm and 99mm see if the error scales perfectly I tried cutting from speed of 0.5m/min to 10m/min exactly the same results.

Carved a lot of 3d stuff on this machine and that's machining for hours not seeing issues there or sign making never noticed the size was wrong until I tried to make an adapter and it didn't fit.

Both X&Y are out by the same amount not sure about the Z.

[Neale]

Sounds good to me. I'll step back and wait for the experts to comment!

[Desertboy]

I measured all 4 parts with calipers within 0.05mm of each other but just not the right size.

[dazp1976]

On the ddscv it's steps per mm

I have 8 microsteps
so 8*200/10 (1610's) for X&Y 160
320 for Z (1605)

Just double checked this is definitely what they are set to.

AM882 has fault protection it should detect missing steps and estop and I swapped all the couplings for these style, I bought the chunkier ones.

27689

so they're rated twice the nm of the motors.

2 4nm in the bottom and 3nm on the gantry, PSU is 70v and 1kva.

Will try and cut 3 holes at 33mm, 66mm and 99mm see if the error scales perfectly I tried cutting from speed of 0.5m/min to 10m/min exactly the same results.

Carved a lot of 3d stuff on this machine and that's machining for hours not seeing issues there or sign making never noticed the size was wrong until I tried to make an adapter and it didn't fit.

Both X&Y are out by the same amount not sure about the Z.

The numbers are really only to get you in the ball park. There's always a slight error on the screws.
Mine is similar on circles. I end up about 0.1mm too small so I just tweek my drawings to suit the machine. I add 0.1mm to inner circles such as do a 32mm as a 32.1mm.
Then outer edges I add 0.05mm on each end (or I can set my stock to leave 0.05mm instead).

This will give you a rough idea on methods of how to increase accuracy using Mach calibration. Or at least to check how close your machine is to see if that is the problem.
https://www.youtube.com/watch?v=XkO5tc-jSxw

[JAZZCNC]

AM882 has fault protection it should detect missing steps and estop and I swapped all the couplings for these style, I bought the chunkier ones.

AM882 doesn't detect missing steps it's got stall detection which is a different thing altogether. It also only works above 300Rpm.

Regards the wrong size parts then if the steps per is correct and you don't have slippage etc then I would be looking to the CAM and the tool offsets.
Does the controller have tool offsets.?

[Desertboy]

What should the rising edge be set to?

27691

I have it set to uprising at moment

[JAZZCNC]

What should the rising edge be set to?

27691

I have it set to uprising at moment

It depends on the controller and whether it looks at the rising or falling edge.

However it's easy to test. Just write some G-code that moves back n forth few hundred short moves, say 10mm, then back to zero. If you have the wrong edge set it will lose a step for every direction change and it won't return to zero. Do this for each axis separately.

[Desertboy]

It depends on the controller and whether it looks at the rising or falling edge.

However it's easy to test. Just write some G-code that moves back n forth few hundred short moves, say 10mm, then back to zero. If you have the wrong edge set it will lose a step for every direction change and it won't return to zero. Do this for each axis separately.

OK I drilled a small hole just outside my normal machining area set that as X&Y 0

then created code to
G01 X10
G01 X0

1000 times doesn't seem to have shifted

just running the Y code now

Will try Z after that.

Can I do something similar to see if I'm losing steps?

Or is there some test code for that?

In the manual there's "Level of Axis pulse signal" what does this mean? Is that the rising/falling edge?
27697

[Desertboy]

This was after 1000 moves left then 1000 moves right and the same on the other axis.

so 4000 moves in total.

The indent was put at G54 0,0 before I ran the code.

Guessing it would be visibly out if I had the rising edge set wrong.27698

[JAZZCNC]

Well, that is pretty much what you are doing so you can say you are not losing steps. However, if you search the forum Jonathan posted an Excel file that will produce G-code to run the machine around then return to Zero.

[JAZZCNC]

In the manual there's "Level of Axis pulse signal" what does this mean? Is that the rising/falling edge?
27697

This will be the pulse timing and I wouldn't mess with it if your not missing steps or losing position.

The fact your parts are the wrong size will be down to either a mechanical issue or simply because the pitch doesn't correspond to the steps per setting. The best way is to command a move and accurately measure the distance it moved. And when I say accurately then a tape measure or even a steel rule isn't accurate enough. For instance, I use linear scales with a DRO to compare actual distanced moved to the commanded. I then adjust the steps per until they match.

The longer the move the better but if you have lets say 150mm length set of digital vernier gauges these can get you very close to perfect.

Edit: One other thing, if these are cheap Chinese screws the pitch can vary along it's length so it's worth taking readings in a few places. Likewise, if you have been using the machine already and cutting in the same spot all the time then there will be wear in this location compared to the unused or less used regions. This is why it's a good idea to move around the bed when cutting small parts rather always at the easiest place to reach.1

[Doddy]

Random thought and I'd appreciate anyone else explaining if I'm talking balls, If you home to 0,0 and manually drop the Z into a sacrificial board, raise Z, traverse e.g. G0X33 (you mentioned a 33mm circle), the drop the Z into the sacrificial board (spindle running of course) then the distance between the left edge of the hole created by the first drop and the second drop should be 33mm. If it is, then your scaling is correct. If not then either thread pitch or steps. If it is still 33mm, and you have all the evidence of no loss of steps then I'd seriously be looking at your CAM, tool sizes and compensation.

[routercnc]

The fact you are cutting circles makes me wonder about the I & J moves, settings for those in the controller (if any), and anything associated with going around corners ?

This is a bit of a long shot but does it do the same thing if cutting out 33 mm square holes (ignoring the tool rad in the corners) ?

I just remember something years ago on I & J radius settings (note: this was in Mach3).

Another option: Is there is a setting for "Maintain velocity (and approximate toolpath)" OR "slow down and follow it exactly" - might be a factor ?

Sorry, just some straws to clutch at.

[Desertboy]

I cut 11 indents they are all out by the same amount ~1mm but the distance between the indents is correct.

27711

So the indent is 49mm and the distance between indents is 51mm. They should be 50mm each.

Over the 11 indents the distance is correct.

Set up 1/2" end mill (Brand new trend bit), pocket no stock to leave.

The top row the clamps weren't tight enough and slipped so cut the bottom row but properly clamped.

I looked through the DDCSV's settings and every tool offset was set to 0.0

[Doddy]

...so the errors are not incremental - so I interpret that as the motor steps, scaling etc are all correct

"Indent is 49mm and the distance between indents is 51mm. They should be 50mm each" - I interpret that that the pockets are undersized?

Post your Gcode output from Fusion. At least for the first two pockets.

[JAZZCNC]

Did you measure the tool.?

[Doddy]

Whoa, random thought - Fusion defaults a number of CAM operations to a roughing cut leaving... 0.5mm for a finishing pass. Have you accounted for this?

[Desertboy]

...so the errors are not incremental - so I interpret that as the motor steps, scaling etc are all correct

"Indent is 49mm and the distance between indents is 51mm. They should be 50mm each" - I interpret that that the pockets are undersized?

Post your Gcode output from Fusion. At least for the first two pockets.

Pockets are undersized, here's the code for 1 pocket 50mm in Fusion 360 I had to rename it to .nc to upload from .tap.

my controller is steps per mm

Microsteps are 8, 1610 ballscrew

8*200/10== 160

I have 1605 on Z so 320

1:1 direct coupling.

[JAZZCNC]

Well a quick look shows that it should cut a 50mm pocket. The last move is at 43.65 and the tool 12.7mm so should hit 50mm provided the tool really is 12.7mm

[Doddy]

Ignoring all the individual line segments...

X lower extreme = 6.35, higher extreme = 43.65. Tool size specified as 12.7mm (6.35 rad), defines a X range of 0..50mm - I guess the operation...

line 231:
G01 X43.650 Y6.350 Z-3.000
G01 X43.650 Y43.650 Z-3.000
G01 X6.350 Y43.650 Z-3.000
G01 X6.350 Y6.350 Z-3.000

is the finishing pass, and should leave a 50mm pocket. Provided that your cutter is 12.7mm diameter.

The code is right (at least that should leave the pocket at the correct size). I'd look to answer Jazz's question on measured tool size. Beyond that, looking at the input to the DDSCV controller (GCode) is correct, you have the configuration of the DDSCV itself that I cannot advise, and the output measured... I'd say the controller is looking suspicious.

[Doddy]

Hmmm, really basic question - you have measured backlash on the axis?

[JAZZCNC]

I'd say the controller is looking suspicious.

I'm not sure it is because it would show error in the distance between the other pockets. The only thing it could be is if it was applying any tool offsets and he says not.!

My money is on the tool being wrong.!

[Desertboy]

I just ran that code to make sure as I did just generate that code and also I just updated the firmware on the controller

27724

27726

[Doddy]

G-Code describes 50mm with a 12.7mm cutter. I reckon your machine is just plain haunted and we should all just self-isolate from it.

The bit that gets me is that it's a very precise 1mm error. But the G-Code is precise and correct.

[Desertboy]

I'm not sure it is because it would show error in the distance between the other pockets. The only thing it could be is if it was applying any tool offsets and he says not.!

My money is on the tool being wrong.!

I'm going to try doing a factory settings reset on the controller in case it's tool offset I'm missing, that I set by accident.

I thought updating the firmware would do that but it did not.

[Desertboy]

G-Code describes 50mm with a 12.7mm cutter. I reckon your machine is just plain haunted and we should all just self-isolate from it.

The bit that gets me is that it's a very precise 1mm error. But the G-Code is precise and correct.

It's always 1mm out

33mm hole was 32mm

99mm hole was 98mm.

[Doddy]

I'm adding noise now to this thread which I don't want to do but I understand (I think) where Jazz is coming from - it's unlikely to be a tool offset or deliberate behaviour by the controller simply because the controller doesn't understand the geometry of the shape being cut - that's part of the CAM to apply the tool diameter offset performed by Fusion depending on the face being machined.

The only thing I can see in the manual are the backlash parameters 437..445 (DS DDCSV V3.1) that would likely have such an impact on behaviour, but even that I'm doubting as it is likely to introduce more steps, rather than reduce.

[JAZZCNC]

I'm adding noise now to this thread which I don't want to do but I understand (I think) where Jazz is coming from -

No No No don't go complicating shit with that it's too consistent to be noise. It would be random and happening all over the place if it was noise.

Still haven't had an answer to if the tool has been measured.?

[Doddy]

Apologies - somewhat out of context. My reference to "noise" is related to babble rather than advice and to the value (or lack thereof) to the continued thread, and not a suggestion at all of electrical noise.

For absolute clarity - I do not mean electrical noise, for the reasoned evidence that Jazz gives.

[Desertboy]

No No No don't go complicating shit with that it's too consistent to be noise. It would be random and happening all over the place if it was noise.

Still haven't had an answer to if the tool has been measured.?

12.68mm I just doubled checked it now.

[JAZZCNC]

Apologies - somewhat out of context. My reference to "noise" is related to babble rather than advice and to the value (or lack thereof) to the continued thread, and not a suggestion at all of electrical noise.

For absolute clarity - I do not mean electrical noise, for the reasoned evidence that Jazz gives.

Ah ok my apologies also, now I read it again in this context I see it, I didn't before and just saw electrical noise and with you being an electronics Wizz and the other electronic bull shit that's going on in another thread I thought OH NO please don't go there...:joker: :loyal:

[phill05]

Have you tried with a different vernier caliper or always the same one?

[Desertboy]

Have you tried with a different vernier caliper or always the same one?

Always the same one but you can see a mm on a ruler which I also tried, the bit is a 1/2" trend router bit, and it's in a 1/2" collet so I think my calipers aren't the issue here.

The pocket even using measuring tape I can see are 1mm undersized.

BUT this gap is meant to be 100cm so the only thing I can think off is the controller is offsetting the tool.


27729

Thinking I might need to connect the X, Y & Z to a breakout board and do a test cut from linuxcnc super slow to see if that shows the same size issue.

[JAZZCNC]

This is a wild shot but suppose must be asked.! . . .You have trammed the spindle haven't you.? Does the bottom of the pocket measure same as the top.?

[Desertboy]

This is a wild shot but suppose must be asked.! . . .You have trammed the spindle haven't you.? Does the bottom of the pocket measure same as the top.?

I can't remember if I did now, I've had the Z off a few times including changing the gantry rails, did I tram it last time?

Will go check shortly.

[JAZZCNC]

I can't remember if I did now, I've had the Z off a few times including changing the gantry rails, did I tram it last time?

Will go check shortly.

Actually, on reflection, it wouldn't make any difference the size would still be correct it's just your pocket walls would be a parallelllllll gram or what ever they are called..:thumsup:

[pippin88]

Have you measured your backlash? You need to check backlash.

[Doddy]

A couple of experiments for you to try.

*** CAUTION: Hand coded G-Code and un-tested. Sit next to your E-Stop!!! ***

27730

This should slowly rock the X-axis by 0.5mm (or 18 degrees on a 1610 screw) - wrap a bit of tape around the x-axis screw with a visible tail and run this g-code through the controller and observe the tape. The G-code has got a feed rate of 10mm/min so my poor maths suggests around 3 seconds to go 0.5mm (18 degrees) and 3 seconds to go back to 0 (0 degrees). It repeats... a few times. No spindle and no z-movement.

This is just to verify that there's no backlash compensation active erroneously or not in the controller. You'll have to eyeball the 18 degrees rotation on the screw/tape.

Remove tape.

27731

This one cuts two pocket outlines - with your 12.7mm milling bit, starts at (0,0) and cuts a 3-tooth comb with a positive displacement on X, 50mm between teeth. After the 3rd tooth it reverses and cuts another 2 teeth offset in Y 30mm back the other way also 50mm apart. This to verify again that there's no backlash effects or compensation in operation.

Sorry, that's all I can think of at the moment.

[Boyan Silyavski]

The easier way to find the edge in the settings is to profile say a 50mm circle with each pass say 0.2mm deeper, so soon its starts to get clear what's happening

50mm circle inside a square is the method i use to test for eventual axis or electronic problems

[Desertboy]

Have you measured your backlash? You need to check backlash.

I ran Gcode to move X to 10mm then back to 0, 1000 times and same with Y and checked position everything seemed good.
http://www.mycncuk.com/threads/13525-My-sizes-are-out?p=115399#post115399

I would have seen backlash with that check right?

[dazp1976]

I ran Gcode to move X to 10mm then back to 0, 1000 times and same with Y and checked position everything seemed good.
http://www.mycncuk.com/threads/13525-My-sizes-are-out?p=115399#post115399

I would have seen backlash with that check right?

Not really no. Even if it has backlash it will still follow the same pattern back and forth so you wouldn't notice.
Have a look at some vids that show how to properly check it.

If your sizes are out by more than say 0.2mm I'd say it wasn't a backlash issue. I've never really seen backlash values of more than 0.08mm which would make a circle smaller by only 0.16mm.

[JAZZCNC]

If you had 1mm of backlash you'd feel it by shaking each axis, it would feel like it's falling off.!

[dazp1976]

If you had 1mm of backlash you'd feel it by shaking each axis, it would feel like it's falling off.!

Tell me about it!!
1 thing I'd say as well is I often use cheap nasty Chinese cutters for roughing through then swap a decent cutter for a finish.
Those Chinese ones can vary in size a chunk.
I can rough a new 6mm 3flute bit using it to finish as well and I won't fit a bearing in the hole.
Then next I'll leave 0.5mm on with the same cutter, swap it for a 4flute Cobalt bit for finishing and be able to just get the bearing in.
That's with my drawings modified where a circle is set 0.1mm lager than I actually want it.

My Benchtop only has 3000rpm at the spindle so I find Cobalt work better for me as I can hog it a tiny bit.
Those Carbide bits are designed for higher rpm and I've shattered a few so there used for finishing only too.

[pippin88]

I ran Gcode to move X to 10mm then back to 0, 1000 times and same with Y and checked position everything seemed good.
http://www.mycncuk.com/threads/13525-My-sizes-are-out?p=115399#post115399

I would have seen backlash with that check right?No, that will not show backlash.

Look up what it is and how to check it.

You need a proper measuring instrument, e.g a dial indicator. You move the axis in one direction into the dial indicator, zero the dial indicator then move the axis in the opposite direction a defined amount. You then check the dial indicator reading and compare to what it should be.

[Desertboy]

I had a blonde moment today, I dug out my old pc which has linuxcnc on it and brought it home to try with the machine I was just going to wire the X,Y,& Z see if the sizes are still out and if so are they out the same amount.

When I got home to set it up I forgot a VGA monitor lol, no HDMI out on this machine.

I need to go work again tomorrow so will have to wait another day.

At the moment I've set the motors to ~3amps on the stepper drivers by jumpers they should be ~ 4amps and they don't get warm even after hours of machining but I will connect them to the PC so I can autotune everything.