Good Day Ross,

Thank you for the response.

I have read this article many times before. I was trying to avoid an exact stop only scenario. I thought that was bad for the machine from what I read. I know cv affects even the z axis. Would lowering the CV to 45 help? The multiple ghosts are annoying. But the ghost all created by the finish toolpath. You can see that here. Photo

Pete, I am afraid that the photo doesn't help me understand what you are trying to explain. :confused:

The slight sheen I see in the photo could be a couple of things.
The far right of object is the roughing area, the left of center is the finish pass area.
Are you sure the part isn't flexing up (bowing) and causing uneven 3D profiling?
This was a very common problem when I was doing a lot of 3d foam cutting and the material slightly climbing up towards the tool bit and causing the appearance of a deeper cut while in reality it was the base material moving.

Sorry Gerald, I am technically deficient when it comes to words to express things at times.

Sean,
The roughing cut was my mistake of not setting the boundry offset in aspire to compensate for the larger tool diameter.

The ghosting of the 3d model that is happening 3x is another story. I just changed my plunge rate to 10 on the Z and set my velocity to 140". The ghosting is a the problem now. Still cutting slow at 33 ipm. Need to find the ghosting problem before worrying about speed. Any input is helpful. This is my first cnc. I may repair them but understanding the fine details is something else of the HMI is something else.

Are you seeing ghost lines/images to the left side only? What is your cut direction?

It is on both sides but closer to the model on the left. Lowering the plunge gave more detail but still have some ghosting. I am using raster along x.

I did have a problem where the Z was bottoming out so I was losing steps and my finish pass was not hitting material, but I think your finish pass is too deep?

In post #204 you mention tool diameter. This was my first thought. Different tool for rough and finish passes?
I suggest trying the same tool for both passes. If the problem disappears, then it is tool specification in the software.

There is no ghosting in the yellow areas?

Does the change in the picture on the red lines mean anything? (This is what I first thought the picture was all about)

The dragon casts no shadow until the cutter reaches the blue scribble?

My impression is that there is no problem in the middle band of the picture, and that you see effects just off the middle band......

Does your finishing cover the whole oval area of the picture, or is your finishing on the dragon only? Did you sand anything before taking the photo?

Red and Gerald,
I ran the program again but with the Z plunge at 10 ipm. The ghosting is diminished but not totally. No it was not sanded in the picture. Was trying to achieve a carving that minimizes sanding in hard to reach places. You are right the problem is in the middle of the picture. On the second run the 0.125 cutter was removing almost 0.100" of material across the hole dish. I only see this with dish carving so maybe the plunge will have to be set very low to stop mach from moving until it has gotten closer to the bottom of the Z until continuing in the x direction. Still trying to wrap my head around the mach controls.

I was thinking the opposite :confused:

Gerald I was referring to the red lines you had indicated. That is the middle of the x but not the y. Sorry, brain works faster than my typing. It seems as if it is the transition from the bottom to the dish on the sides of the dragon and I have know idea what is going on around the red line and why it is missing the bottom of the convex shape.

What about motor tuning. How does acceleration and velocity affect the cut quality?

On another subject, the upgrade to water cooled spindle. If someone was to ask the difference in sound compared to a PC7518, I would tell them to just buy the spindle. You can barely hear it running and the faster it turns the quieter it is. My Jet dust collector is louder than the spindle cutting and the Jet is 85dB. Second listed but most important, dust collection. A router is air cooled. The PC7518 is an awesome router but the amount of air it moves it will push the fine dust through your dust shoe and all over the machine. Since the upgrade to the water cooled spindle. The dust collected has doubled. There is no more dust collecting on the machine or on the table. Only the occasional larger chip that launches from the shoe opening for the spindle entry. The dust collection alone is worth the upgrade. My total cost to upgrade was $1200.

Hi Pete

My Exact stop suggestion was a diagnostic test certainly not a suggestion you use it permanently.

Maybe experiment with the types of of 3D roughing and finishing passes are you using.
Maybe using a 3D raster roughing path might help.
The Z level roughing makes the little islands while the 3D raster runs along the X or Y jumping the Z constantly up and down to follow the contour.
I have seen many of these 3D raster toolpaths complete very well.
Try that followed by a raster finishing path.

When in doubt slow down the feed rate and start making the tool stepover smaller until you get what you want.

No solutions only suggestions but somewhere to start that has not been discussed in the previous posts.

regards
Ross

Ross,
Thanks for the input. I spent the past 2 days trying to find out how to minimize this. This is what I have found, uh, well, nothing really. The toolpaths are raster x, found Aspire likes to leave a notch when using offset. Spoke with a gentlemen from Texas and he gave me some things to try. He better explained about how the Z looked like it was going to deep. Amazing how when you can talk to someone rather than type you can get a better understanding of it. I have tried even slowing the velocity down to 10 and accel to 6. This forcing mach to run rapid but move at Z velocity at the height changes. Still have the flat spot on the oval. It was neat to see how the changes affect Mach3 control. I wish there was a way to set Mach to understanding I want the Z speed to be 10ipm while x and y 80ipm without doing it in motor tuning. Looking at the Gcode the F sets the feedrate for travel. I did not see a code reference to set a locked feedrate for one axis. However I do not know if that would help.

Since I am using the PK296A2A-SG7.2 for all my axises, I would think that the Velocity on x would be more than the amount of y and z. However I have x and y the same at 498.02 and 25 acc. Z is now set at 300 and 40. All the tests came out relatively the same. I added more spring tension to Z. Was a little light compared to the rest of them. Need a better mounting spot for the spring or a longer spring. Using a cable tie to the spring now for added force in the meantime. Time will tell me what to do but for know I am stumped.

Interesting

I tune the motors to the job and just kind of accepted that was the way it was done.
The often made statement that the machine is "now tuned perfectly" never sat well with me.
Unless it just did the one job over and over (as is often the case for a production machine).

Don't do much or even any 3D of late but I'm certain my current motor tuning would stink for 3D.
The reason this is so is that they are tuned mid level fast with a nice smooth (read slow) acceleration.
If I was to run the machine and particularly the Z for 3D then the Z move would be over before it got to top speed.
No use telling the software to go a certain speed if it is never going to get there before changing direction again if you know what I mean.

Suppose what I am saying here is divide up your job types and store an xml file away that tunes the machine for a particular job.
Mach3 stores away the motor tuning in the xml files so it is a simple as loading the right xml once you have sorted your job specific tuning.

In practice I am far from that organised and just tune the machine each time.
The exception here is my shaping machine tuning that I keep as a xml on my PC.

Another way of thinking about motor tuning for you perhaps Pete.

Regards
Ross

Ross, thanks for the post.

Gerald,
I narrowed down the problem with the uneven spacing of lines. You mention in your post about flex. Well that got me to thinking about the home switches. Ends up the X switch was not set correctly to the A(I need to change it to B) switch. It was referencing to a twisted home position. The X switch was for one, too high (prox switch) and two, not in the correct spot. Just ran a photocarve with 0.030 line spacing and it is almost dead on. Thanks.

Never would have picked that Pete, well done.
For your reference the gantry is squared by referencing to the hard stops and not the home switches.
Either drive it up the stops with the limits off or pull it up against the stops and turn the motors on.

Regards
Ross

Ross, I knew about the about the stops but I also was told about the motors off and to leave the motors off for a couple minutes to release any residual energy in the circuits and the motors.

One thing I have noticed looking back through the pictures is I did do a couple of dish carvings with offset. With it no ghosting appears but the notch appears when aspire moves up in the dish. Raster gives the ghost lines because it is going to deep. Obviously the ghosting is easier to sand out.

Ross, Sean, Gerald and Red,

This is what I have found so far.

The steppers I use have a gearbox, me not thinking, all gearboxes have backlash. They have to or they will destroy themselves. I should have thought of this because of my occupation. I checked for backlash with a dial indicator. Found 0.010" backlash. I should have remembered this from the specs when I spoke with Oriental Motors. I vividly remember him saying 0.9° of play. That is roughly 0.0118" across my 1.5" pinion when drawn up in cad. I set up the compensation backlash in mach and tried the piece again. All the ghosting and flats are removed. Not used to seeing a stop-go machine but in the end the parts will be better. The only problem is the first bump compensation is almost 0.003" but the moves are dead on after that. With standard V-carving I never noticed it and with raised models I never saw a problem. Must have just been the way the programs were generated. Sometimes you need to remember your basics.

Interesting note about the backlash on the z-axis.
Maybe, just maybe a belt drive for the z-axis only might be in order. This would speed up the cutting process. I have experienced how much time the Backlash Comp profile adds to each move....painful to watch on a huge project.

Thank you for the feedback. Well noted.

Was looking a this link. Have tested it and you do hardly notice the backlash compensation.

That bad thing is that all axes have the gearbox reduction and I tested all axes and they are all exactly the same amount of backlash. Some things require better planning. I often debated about a belt and pulley versus gearbox. Never thought about it. Now I am thinking maybe the other would have been better.

Pete - it is like reading a mystery novel :D

That link I attached previously about CV settings actually explains "in English" what on earth shuttle accel. does.
As per a lot of Mach3 settings not all that intuitive.
To summarise the Hoss video settings, he set the Backlash Speed % of Max to 100% and changed the Shuttle Accel. settings in Config, General Config.

Got to think out loud though, you are using a very common and high quality motor.
While these settings and the backlash compensation work, still does not explain what so many others have been able to produce good 3D without these setting enabled.
While I have gone the belt reduction path I would not rush to the conclusion that your choice of the Oriental Motor stepper motor was a poor one.

Regards
Ross

Understood Ross,
Just frustrated is all. Have spent a good deal of time on this and I know that other have had good results. This is where I am at a total loss. Using the dial indicator, I first saw the free steps and it was moving per step at 0.0003". It was not until the DRO was a 0.006" that the steps started to show and move accurately at 0.0003" per step. I repeated this many times. So I thought "well it is probably only the Z" but curiosity got the best of me. So I checked X and Y. They both have the same issue as the Z. So I looked at the radial play.
Do I think the Motor I have is a poor motor...Absolutely not. Does it give good results on what I have asked of it...Yes. Will it give me the pure results I would like in 3d, not with the specs the way they are. It would not be a bad carving but not as sand free one either near perfect one either.

Too bad I can not compensate for this another way.

I am interested in what number you actually put into the backlash distance and speed did you use. I am not sure how to calculate this.

I never thought of using it but if it helps I am willing to try it.

Thanks

Nils,
I am looking at what Ross refered to in the CV settings first. I will explain calculating backlash last.

CV notes copied from HERE
"Shuttle Wheel Setting (Shuttle Accel.____ Seconds)
Determines how much time is allowed for the backlash takeup movement to take place.
For my servo systems I set this to a VERY small value (0.00001). This will prevent the
backlash motion from affecting the smoothness of the machine because the step pulses
are sent out as fast as possible (to the limit of the kernal speed). A large number may be
required in stepper systems to prevent lost steps."

To calculate backlash move the axis in one direction only and stop. Set up your dial indicator and set to zero. Open your jog screen and set it to Single Step and change your mode from Cont to Step. Change your step increment to the minimum value your stepper makes. Mine is 0.0003" yours my varies well be different. Now move the axis using the corresponding button or key in the opposite direction you originally travelled. Keep pressing the key until the dial indicator actually moves the correct distance it set to move. I was using a 0.010" check. I hit the key until it moved 10 thousandths of an inch on the dial indicator. I took the dro setting and subtracted the 10 thousands. Mine was 0.0098". Normally you can just wait until the needle moves and subtract the two but in my case the needle was moving ever so slightly that the first complete jump was between 0.009 and 0.0011 on the dro and 0.004 and 0.006 on my dial indicator. That is why I used a ten base.

Ross,
I love your responses. Straight and to the point with your comments. I am like that so it is appreciated. I think I will have use the backlash comp for the time being. I have not noticed a huge difference in a 40 minute carving. Adds a minute amount of time. Will be looking at upgrade options for when the compensation starts to cause excessive wear in the gears. Will give me plenty of time to work out the finer details of belt driven systems.

How do you change the title of your thread????

I do it .... slowly it seems lately :D

Mike, a change to reflect the current status is would be greatly appreciated.

Dust shoe info
 

Has anyone used natural horse hair for the brush on the dust shoe. I find some finely grooved wood is affected by the stiffness of the nylon bristle. I also feel it would kick up less fine dust.

What are your opinions?:rolleyes:

So. I was cutting out the deer in the forest scene. After it completed it did a v carve. Next was a profile carve. When it got there, the steppers would overrun (rapid loss of steps) when it rapid move to plunge position. I must have played with it for 2 hours trying to get it to run but it did the same exact thing. Tried shutting down mach, the computer, everything. Still could not start from the line it quit at. Out of desperation, I loaded another previously run program. And it cut air fine, tried a different one, ran fine, reloaded the original deer program and it overran again. Went up to the computer and output the remaining toolpaths and took it to the machine. Loaded it and it ran fine and finished the plaque. I have no idea want was wrong with that part of the original program but it definitely did not work.

Changed over Z axis to 4:1 belt reduction. Used a PK296-F4.5A Oriental Motor stepper wired parallel. Used 72 tooth timing gear and 18 tooth gear with this belt. Bored out the gears to fit the designated shafts. I reviewed the drawings and other designs here but they did not fit my layout with my dust collecting mount. I needed a unit when the spur gear was engaged that it was straight up and down. I also used 2 idler gears to ensure maximum engagement on the small timing gear. The spring attaches from the top post on the gear reduction box. Attached the drawing I used in case anyone may need this in the future. I got a lot of help from Mike so a big thank you there.

Forgot the tension adjustment plate. Sorry.

Pics

Looks about perfect to me.
Well done.

Thanks Sean.

Just cut out another 3d model in a dish. Problem is now resolved. Definitely has a different sound than the gearbox steppers but it doesn't have backlash.

Success :)

Regards
Ross

Pete

Excellent drawings. Thanks for the details.