Reply with QuoteThe model came out the correct size, yes?.
Was it double the size it should have been by any chance?.
stepper speed some clarification required
Hey G'day folks,
Just a question regarding speed, I currently have my dm542 stepper driver resolution set to 1600 since replacing my old drivers. My cnc runs what I would say quite slowly.
eg pic Im posting.
I took a 3d model that I made with my resin printer and converted it to a bas relief.
I know how to control the speed of my print there are various things I can do to make it pint faster. eg decreasing the lift off time, increasing the resolution from .5 to 1 micron etc, the 3d print took 11 hours to do at the settings I had, I could have nearly halved that by doing other things but I wanted the best quality for a test I could achieve so 11 hours was good. Model hight 160 mm.
The carving took over 5 hours 320 x 190mm 1.5mm ball nose single pass no roughing done in cypress, (first time I've used cypress personally don't like it much).
My question, is my resolution to small? That carving I should be able to do in 2.5 hours half the time. I can increase the setting in uccnc to +200 the speed up does not work, I can go negative to say - 20 and my cnc will slow going about 100 has no positive effect.
I've been using uccnc for a number of years now I still really don't know too much about it.
I used Mach3 previously and going + over riding speed worked but not the same with uccnc.
Any information gratefully received, trying to save myself a little time for more real life stuff .. possibly lol.
Cheers,
Steve
Similar Threads:
Re: stepper speed some clarification required
The model came out the correct size, yes?.
Was it double the size it should have been by any chance?.
Re: stepper speed some clarification required
What made you think it should have gone twice as fast? With a 3D carving like that, increasing the feed speed doesn't have much effect. The problem is that you've got a whole lot of tiny sideways moves, with constantly changing vertical moves interspersed, so that no single move can get going very fast before it's over. Maybe if your system could serve up each move faster, and the acceleration was higher, you'd make progress quicker, but that's not affected by feedrate.
[FONT=Verdana]Andrew Werby[/FONT]
[URL="http://www.computersculpture.com/"]Website[/URL]
Re: stepper speed some clarification required
Acceleration is the major limitation in 3D carving.
You can change your step over, however that will affect your detail (similar to changing layer height in 3D printing)
Re: stepper speed some clarification required
Model was the right size, not double
Re: stepper speed some clarification required
Well it could be faster, the machine is running too slow. I understand there are a lot of sideways movements the more detail the slower it can get .. I think 5 hours is excessive. which is why I am asking the question.
Re: stepper speed some clarification required
Pippin I understand that, theres no need for me to alter the step over. When I was using mach3 I could bump the speed on my carving from 100 to 200 and it would move, yes a small amount of detail may be lost but I was happy with that, not all carving need to be 100%. With UcCnC I can crank from 100 to 200 and there is no difference in movement. That's why I'm asking the question what would be limiting the speed?
Originally Posted by curiosity22
Well. If the 2.5hrs you mentioned was calculated during simulation in cam. Then I would agree with the idea of it being down to acceleration / deceleration of the steppers.
This is one thing that the cam won't take into account.
What are your settings at?.
What are the steppers?.
What voltage are the drivers running on?.
When I first started as hobby I had one of those ebay 36v 'kits'. Accel was rubbish, kept stalling if raised. I eventually went to bigger drives and higher voltage and now I can set really high values, practically stopless.
Re: stepper speed some clarification required
Hey G'day,
Thank you for taking the time,
I've just upgraded my drivers to the DM556T settings at 1600, steppers are 24H290-35-4B (nema24) running at 48v.
Just as a by the by I reinstated Mach3 for a test run, when I increase the % over 100 cnc runs faster it responds to the increase. UCCNC not doing the same, if I remember correctly I had a similar issue with Mach3 many moons ago and it was something to do with "exact stop" a setting within Mach but buggered if I can be precise on that its been a number of years now since I've played with Mach3.
Cheers,
Steve
Re: stepper speed some clarification required
"Exact Stop" means the movement will be from A to B, and it will STOP at B. Then it will make the next move to C, with a STOP at the end.
As you can imagine, this can be very slow as the axes never get up to full speed. Increasing the acceleration might help - a bit.
If you turn Exact Stop off in Mach3 the path planner will try to get very close to the point B, but it will allow for a tiny error as it 'moves on' to the next path segment. The motion becomes essentially continuous. The difference in speed can be huge, and you will also 'lose' the continuous shuddering which came from all that Stop/Go.
I do not know UCCNC, but surely there must be a way of doing the same?
Cheers
Roger
Re: stepper speed some clarification required
Hey Roger,
Thank you for taking the time to reply, I found that out about Mach3 a few years ago as I had the same experience I'm having today. I'm still trying to identify where exact stop is for UCCNC or the equivalent is. If anyone knows would be great. Yes, the continuous shuddering drives me nuts at times lol. Considering the majority of any work I do with my cnc is Bas Reliefs.
I'll send an email to Balazis and see if he can't demystify it as well.
Cheers and ty again,
Steve
Re: stepper speed some clarification required
UCCNC Users Manual, page 21
Interpolation mode selection:
This parameter selects how the trajectory planner executes the motion.
There are two modes, the exact stop mode and the constant velocity mode.
These two different modes can be also selected executing the G61.1 (exact stop mode) and G64
(constant velocity mode). When these codes are executed the selection on the screen changes
accordingly. When a G64 code gets executed the parameters for this command are read from this
screen settings.
Exact stop mode:
This is a trajectory planning mode. In this mode the trajectory planner follows
the motion path positions exactly. The machine axis accelerates at the beginning of each segment
and deccelerates at the end of each segment. This interpolation mode is adviced to set if close
tolerance parts are manufactured. The position error is always zero with this interpolation mode.
Constant velocity mode:
This is a trajectory planning mode. In this mode the trajectory planner is
interpolating to the set feedrate, in other words the trajectory is planned looking ahead in the motion
path and trying to keep the feedrate constant on the set feedrate.
For this mode to work some additional parameters needs to be defined which are discussed in the
followings. The constant velocity mode is adviced to be used when high speed machining is
nessessary for example 3D artworks are machined. This mode can also be used for close tolerance
parts machining, but the tolerance parameters for this mode must be set correctly to force the
motion planner to not make higher position errors than what is allowed for the workpiece.
There is always a tradeoff between machining speed and precision. The higher the allowed
machining errors are set the faster the job will be finished, because the motion planner has more
space for optimising the motion, however the less the workpiece precision might be.
Search, read, and you will find.
Cheers
Roger
Re: stepper speed some clarification required
Cheers Roger, I'll have a look at my GCode and see what's being executed. I'll be my bottom dollar you were right I have it set to exact stop mode. What I need is obviously Constant velocity.
Thank you for taking the time,
Steve
Re: stepper speed some clarification required
Hum - a 1.5 mm ball nose cutter?
How many did you break?
Normally, one starts with a much bigger cutter for the roughing out, then switches to a finer one for the details.
Cheers
Roger
Re: stepper speed some clarification required
Hey Roger G'day,
I broke none lol... I have pretty much given up on roughing at all for any of my 3d carvings. The only time I will sorta do a roughing pass is just one row with an end mill just to give the ball nose an opportunity to start. As you know they aren't the greatest in cutting a channel. Otherwise if its a 3d carving from the edge I don't rough at all thorough waste of time.
I should have stated that I use a tapered ball nose it has a cutting edge of 30mm eg https://www.ebay.com.au/itm/25258646...frcectupt=true
I have done about 10 carvings with the one bit so far and its still sharp and going.
Most of my carvings rarely exceed 30mm depth which is ok for me. If I do a carving that is deeper I'd look for a tapered ball nose with a bigger cutting edge.
I used to always do a roughing pass before final pass, It used to annoy me that only a small portion of the tool was used so did a test carving with a single pass, never looked back.
Here's one for the bigger jobs.. https://www.ebay.com.au/itm/26276203...sAAOSwal5YCX~9
Cheers Steve
Re: stepper speed some clarification required
OK.
Those tapered cutters are MUCH stronger.
And I guess the wood is a bit softer than the aluminium alloy I am often machining. I have to work to about 0.01 - 0.02 mm with it.
Cheers
Roger
Re: stepper speed some clarification required
Hey G'day,
Oh for sure, 0.01/.02 that's reserved for my 3d resin printer lol.. I've not yet tried to work with aluminium but I would like to have a crack at it. What I would like to try is cutting some gears, I have a rotary axis set up at the front of my CnC any advice on a cutter that I could use with my spindle to accomplish this? I really would like cutting some metal gears (brass/aluminium) instead of using Perspex ones I cut with my laser or 3d printed ones.
Cheers,
Steve
Re: stepper speed some clarification required
Somewhere or other on CNCZone there should be a thread started by me on cutting GT2 pulleys. I have made them in no less than three different ways.
#1: Flat slab on mill table and trace around the contour with a 1 mm cutter. Just XY movements with a slow creep down on Z. Very slow, and only suitable for thin gears as the 1 mm cutters are not long.
#2: Machined a profile cutter for GT2 from hardening steel and then used the A axis to cut the teeth. See pic 7324.
#3: Used a 1.1 mm ball nosed cutter to make multiple passes through the teeth to shape the profile. See 7572.
These required custom g-code programming: no CAM.
The aim was to make GT2 pulleys to upgrade the axis drives on my CNC. See 7331
Cheers
Roger
Re: stepper speed some clarification required
I'll have a search for your thread, the first pic, whats the cutter called and at a guess its designed to fit in a standard spindle? So that's cutting on X in the dead centre middle.
Thanks mate,
Steve
Re: stepper speed some clarification required
the first pic, whats the cutter called and at a guess its designed to fit in a standard spindle?
The cutter itself is the profile cutter I made, from the details of the GT2 profile in Gate's patent. The cutter was machined in the lathe to get the profile, then half of it (to the centre line) was removed to make the profile cutter. Then heat treatment and finale polish with a CBN wheel. Hours of fun . . .
As for the shaft - a bit of hard 16 mm steel rod. And yes, on the CL.
Um - was the article on CNCZone or on Artsoft? Can't remember.
Cheers
Roger
