Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Sage on March 05, 2009, 11:34:58 AM
-
I'm using the Wrapper sotware to machine some text onto a cylinder. Although I've set all the parameters in Mach according to the wrapper software HELP I can't get the Mach toolpath display to show a cylinder with the text as it says it should in the wrapper help. The toolpath is just some sort of flattened X,Y,Z display. No A axis shown. I think the machining is going to be correct judging by air cutting movement but it would be nice to see it properly in the toolpath.
Ive set Mach:
Config/toopath/ A-rotations checked and Axis of rotation X checked.
Confg/general config/ rotational - Rotate 360 rollover unchecked.
Anything I'm missing.
Sage
-
I dont know much about the 4th axis but wondering if you have A axis checked as Angular?
Hood
-
Hood:
Yes A-axis is set to angular.
One strange thing is I went back a few minutes ago to play abit more. I loaded the file again and it showed up fine as a curved surface in the small toolpath display and seems to rotate fine as I ran the code. Then because it was a bit small I went to the big toolpath diaplay and even after regenerating it there was no way to get it to show properly. I went back to the small display and now it too was screwed up. I shut Mach down, started it again and check all the settings and still I can't get it to show up properly again. Only that once it showed properly.
The file is attached. Maye someone else can comment. It is the letters TSME. It should show on the toolpath as a slightly curved toolpath so it may require some pushing around with the mouse to see it all properly.
Thanks
Sage
-
This is how it shows up here, does that look correct?
If you want to attch your xml I will have a look.
Hood
-
I am not at the computer I have doing 4th axis right now so can't check all I have set.
However I do know that the diameter that is set in "Rotation Diameters" affects how it is displayed in the toolpath window.
Not sure if this is intended but it does.
Greg
-
Hi, Sage
As Greg stated, Do you have a value set in Setting's, Rotation Diameters for the A axis.
Chip
-
hi Sage,
using your settings, here is what I get...wraps around too many times :P
I've been interested in 4th quite some time, and with your setings, you have shown me how to get this far! Almost
there!
Thanks, Glenn
-
Sage
using ver 3.043 here.i posted my settings.your file looks good here.i took the liberty of editing the rapids in the file.but that had nothing to do with the view.
bill
-
here is the rest
-
Thanks everyone:
docltf:
I set what you have stated and it looks fine now. Now all I have to do is remember the settings.
What else will the rotation diameter affect ?
The next question is:
My rotary axis work fine for other purposes so far - accurate and reliable. The parameters for it are:
300 oz/in NEMA 23 200 step motor with Gecko set for microsteps (2000 steps per rev of stepper). Fits on the table and still allows normal mounting of table to mill without motor interference.
The rotary table has 90:1 ratio
I calculated the following settings for motor tuning to balance missed steps on acceleration and enough power under load.
360deg / 90 = 4 degrees per rev
2000steps for 4 degrees means 2000/4 = 500 steps per degree therefore settings are:
Steps per = 500
Velocity = 669
Accel = 9
For normal use the rotary table is fine although a bit slow on G0's but I find it missing steps under load if I speed it up. I'm not in a hurry. But maybe I've missed something here.
The problem is with the code from the wrapper program. It has only a fixed F60 which is rediculously fast for the X axis and too slow for the A axis. 60 for A is almost not moving.
For the lnes of code with X and A on the same line it actually results in a feed of about F2 for the two combined because the A movements are slowing down the X. F2 is about what I'd like to use for a 1/16 cutter.
Editing the code to put different feeds for each line is the only solution but not reasonable. ( I tried it).
So the question is (after all that):
Is there something I've done wrong with the settings for A or is there something else that can be tweeked to make the A axis work better for wrapper.
Sage
-
Sage
have you tried a higher velocity on your A axis ,something like 2000 and make your pulse width wider.what are your settings for the X and Y. i did a air cut with your code today on my machine
and it ran well.
bill
-
Running in air might be fine.
How's the balance between X speed and A rotation speed for you?
60ipm for X is crazy fast for a 1/16 cutter.
Put some metal under it and see what happens for you.
I tried faster A velocity when I first set it up but the motor was losing steps on start up on G0's. I could try tuning the acceleration a bit to compensate. I somehow doubt there is going to be a stepper speed that s going to suffice with the rotary motor working into a 90:1 gear ratio compared to the X and which are just driving ball screws.
My X and Y are set to 20000 steps per and a velocity of 50 ipmin. That gives me a G0 of about twice what I can turn the handle (mill drill) at which keeps me out of trouble.
As a test I purposly de-tuned my X axis to slow it down. That helped balance things for the wrapper code but obvioulsy that isn't a good solution. Or maybe it's all I can do to have a separate XML for this application.
What kind of rotary setup do you have??
You mention setting pulse width wider. Where is that done? I'm scheptical on that becuause I use Gecko drivers and their going to drive the motor how they see fit. I'm not losing any pulses from Mach to the drivers. That interface is solid.
I just think I'm driving the motor too fast for it's abilities to overcome the 90:1 ratio compared to the direct drive of the X axis.
Sage
-
Sage
the air cut i did looked pretty smooth and balanced.i did not have to change the feed rate in the code .my machine is not set to operate that fast.so it just ran at my maximum settings.I also use small cuttters at times,the smallest
is .0075 ,have not killed one yet,but have killed plenty .03125 playing with differant feed rate for differant materials.the A axis on my machine is 600 steps per degree.the X axis is 3200 steps per inch.in your post you mention your
X axis is 20000 steps per.does that per, mean inch?it might be your X axis is maxing out your A . try reducing your microstepping on X by half.the pulse width is for time balance between driver and computer.you will find it in motor
tuning.when i first set my A axis up the motor would not act properly.the motor was the same as the motor on Z axis .X Y and Z were running well. drove me nuts! so i set the A axis as spindle in ports and pins.then started to play with
pulse width running the motor as a constant speed spindle.the motor smoothed out and acted properly at a pulse width of 9 . my old setting was 5 and i thought my machine was pretty smooth.now it is real smooth.between mach,
my computer and the drivers ,setting my pulse width at 9 runs it the best.if i have to use my backup computer that pulse width has to be set at 3 to do the same thing.
bill
-
I have no control, over the microstepping. The Gecko drivers are fixed at 10 microsteps per input step pulse. Likewise the pulse width makes no difference with a Gecko. It's an edge triggered device therefore pulse width will have no effect.
20,000 steps per inch is not unreasonable for X and Y.
I have 0.2" per revolution ball screws. So the math is.
200 step motors x 10 microsteps = 2000 steps per revolution.
1 revolution is 0.2" of table travel.
0.2" / 2000 = .0001 or 1 tenth thou per step (10 steps per thou). I wouldn't want a step any bigger.
The A axis is not being slowed by X. The contrary is true. In a combined instruction the X is slowed down considerably waiting for A.
Consider:
G0 X1 A1
where X is 1 inch and A is one degree. Being that the two are on the same line of code they must complete at the same time to form a diagonal, therefore the X has a whole inch to move and the A has only one degree. You can figure out the the linear distance of one degree on a 6" rotary table as 6 x 3.1415 = 18". 18/360 is only .05 inches. X must be slowed down about 20x to be linear with A. (1/.05)
This has been proven when I run the wrapper code. Combined lines wi X and A don't need modification, X-only lines need a big reduction in the feed rate and A only lines I can practically run at G0 speeds since My A is so slow.
Let me play around with it a bit when I get some time. Maybe I can improve the A performance.
Sage
-
Hi, Sage
Using the G-code you posted, Wouldn't using F60 for your cut speed be an excessive value for cutting with a small cutter anyway.
Set it to a realistic value for the type of material your cutting, Make sure your using "Diameter for Federate" in Config, Tool-Path.
I think your masking Mach3's ability to work as it should, Tune your Velocity's & Acceleration's with G0 moves till they skip then back them down a little.
Would think your A axis Acceleration could be higher.
Just Thinking Hear, Chip
-
I didn't program the F60. Wrapper did.
You're missing the point. I guess I tend to provide more info than people care to read.
YES F60 IS excessive for X moves but it's also - at the same time - too slow for A moves given my current A configuration.
There is only one F speed code programmed in the code produce by the wrapper program.
For me, the speed resulting from G0 is closer to a desireable speed for A moves and a 1/16 cutter (just bit fast).
I agree that it might be possible to modify my A configuration BUT as I already mentioned I went through the process of tuning it until it skips and backing off a bit. I doubt there is any all encompassing F speed that will satisfy my hardware arangement.
I haven't really st down and thought about it too much. I'm sort of busy right now. I'll have to ponder it more.
I'd like to hear from someone else using a 90:1 ratio rotory axis and what motors and setting they have.
Sage
-
Sounds like the bottom line is that you want different feedrates for the rotary and linear axis. Is that correct? I don't think Mach3 can do this. It tries to move the tool at the commanded feedrate, no matter where it's going. The A diameter and Use Diameter settings allow it to do this.
The problem seems to be that your A axis is just too slow.
-
Mach is doing a good job slowing the X down to accommodate the slow A when X and A commands are on the same line. This is absolutley required since otherwise a proper diagonal would not be possible - so no I don't WANT (or need) different feed rates when moving in X and A together but I do NEED a different rate for the lines with separate X and A moves.
I'd still like to hear from someone with a similar setup (A axis 90:1) and what settings they have for A axis and the results they get running the sample program. I can't see there being a single feed rate that can possibly work for both X and A.
As I mentioned before I have no problems with A the way it is. Until now I've never had a reason to move X and A together in sync. I've cut gears before but that's only a position A and then cut X sort of function and it makes no difference how long A takes. Since the two commands are always on separate lines of code I can adjust the Feed rate for all A position commands.
Let's hear from others using rotary tables .
Sage
-
PS> What is this "Use diameter" setting you are mentioning. I seeit in the settings and have it checked but where ids the diameter of anything entered in a mill program? SO what is Mach using to calculate anything referenced to diameter?
Maybe someone can explain what Mach is going to do with (or without) such information.
Sage
-
You enter the diameter of your part on the settings page, and Mach uses it to caclulate feedrates.
-
Thanks for all your help on this people. I think I'm finally getting the picture.
I hadn't noticed that setting the diameter in the settings page, in addition to making the toolpath display proper, does affect the feed rate for the A axis. Perhaps I didn't have all the settings applied at the same time in the various places.
I have only looked at the tool path display but the speed of X and A now appear about the same. I'll have to see what it actually does on the machine.
So - I presume what Mach is doing when applying the diameter factor, is managing the feed of A by inches per minute based on calculating the circumference of the part in inches rather than applying the feedate number as the usual degrees per minute. Is that what's going on?? Seems so.
This looks more manageable by a single feed rate in the code.
I'll have to try it out on the machine later and see what the movements look like.
Sorry for being so dense on this issue. It was difficult to see how all the pieces fit together. :P
Very cool !! 8)
Sage
-
Sage,
Just wanted to know if you ever got this figured out?
I'm starting to actually cut with my setup (72:1 sherline rotary table) and I get the same results as you were getting, super slow rotations and super fast x movement on straight segments.
Thanks,
Dave
-
G'day Dave
Did you pick up on the "Use Diameter for Feedrate" setting on the toolpaths dialogue box?
This will try to adjust the rotary axis feedrate to account for the diameter of the job.
The other issue is that often the gearing of the rotary axis simply will not allow for the axis to rotate fast enough to give 60 ipm cut speed on a 2" diameter job.
As the rotary axis speed bumps up against the max steps per min for that axis, Mach will slow down the other axis to achieve a coordinated move.
My rotary axis will only achieve about 4 rpm which translates into about 25 ipm at 2" diameter.
So no matter what feedrate I command in gcode, feedrate will sometimes be limited by that factor. Depending on the move segment.
Greg
-
Hi Guys,
I'm trying to find a less expensive way to make a rotary table,
would a 425ozstepper turn something like this, or would this worm gear have
lots of resistance? They seem to be fairly cheap compared to some of the rotary
setups I've seen associated with cnc.
Thanks, Glenn :)
-
.....would a 425ozstepper turn something like this, or would this worm gear have
lots of resistance?
That probably depends how fast you want to turn it. Steppers lose torque with rpm.
I made a rotary axis using a similar gearbox. See this link,
http://www.machsupport.com/forum/index.php/topic,6158.0.html
It works pretty well for a router. Probably not backlash free enough for a mill.
However I do believe it compares reasonably well with some of the rotary tables hobby users employ.
Greg
-
Glenn,
An easy way to check torque requirerments is just turn the axis wiith a torque wrench and
see what the readings are.
Look around, you can find them used in in-oz.
RICH
-
Greg,
Thanks for link and helpful information, I see that your red box is what I am looking to use
and I have found one in ebay at a reasonable price. :D
Now that you have been using yours with great success, if you could do it all over
again, would you choose a different ratio, or are you satisfied that the ratio you chose is
best suited to your application? (which is the same requirements I will be seeking!)
I ask this because there are several different ratios to choose from, and 10:1 looks good
but will a stepper turn it? ???
RICH,
Thanks for the tip-
I am going to have to get a torque wrench! This would be very helpful. :D
Glenn
-
I see that your red box is what I am looking to use and I have found one in ebay at a reasonable price. :D
It would not want to have any wear in it. There is no way to adjust for that.
if you could do it all over again, would you choose a different ratio, or are you satisfied that the ratio you chose is best suited to your application?
I think mine is 40 to 1. I got got it for almost nothing. That is why I used it. Mildly surprised it works as well as it does.
Not sure about the ideal ratio. It is fairly stiff. Made for much higher loads than it is getting. Large bearings and seals and thick oil, all contribute. 400 oz stepper is only just enough.
Greg
-
Greg,
Now I'm not so sure about this ...I wondered about the large loads this
box was designed for; I can see (now that you bring it to light), how the large gears and bearings and thick oil would rob my little
stepper of most power- just to turn the gears. So I may not rush into a $50. purchase yet, until I can somehow actually test it's
torque with a wrench(Thanks RICH), the difficult part is, a person can't test things from mail order or ebay.
I will generally only be using 4th axis on items 1.5 " or smaller, I would like to put design or customers name
on lower barrel part.
Glenn
-
G'day Dave
Did you pick up on the "Use Diameter for Feedrate" setting on the toolpaths dialogue box?
This will try to adjust the rotary axis feedrate to account for the diameter of the job.
The other issue is that often the gearing of the rotary axis simply will not allow for the axis to rotate fast enough to give 60 ipm cut speed on a 2" diameter job.
As the rotary axis speed bumps up against the max steps per min for that axis, Mach will slow down the other axis to achieve a coordinated move.
My rotary axis will only achieve about 4 rpm which translates into about 25 ipm at 2" diameter.
So no matter what feedrate I command in gcode, feedrate will sometimes be limited by that factor. Depending on the move segment.
Greg
Hi Greg,
Thanks as always for chiming in.
I believe I have that checked but I will look to be sure when I get out to the shop.
I'll report back soon - :)
Dave
-
Ok, just an update, I did NOT have "Use Diameter for Feedrate" checked and while it definitely smooths things out much more, there's still a difference in feedrate ratio from the A to the X but , as mentioned above, I do believe that it is due to my table ratio being 72:1, but it works great and I'm very happy with the whole setup.
Thanks again, Greg and thanks to Sage for starting this thread to begin with- 8)
Dave
-
Hello Glenn,
That Cobra gear reducer and other like it are probably not what you want. The input shaft at the motor end is totally UNSUPPORTED by any bearing, if it's like the ones I have. And it looks so in the pic. They are designed to be bolted to the face of the motor and aligns itself to the motor shaft and the motor bearing. There is nothing in the reducer but a seal.
You could make an adapter with a bearing but it would be a lot of work.
I'd look for one with 2 bearings on the input shaft.
Been there....
RC
-
Sorry for taking so long to get back with a reply but there's been a lot of activity on this topic in the last day. That's good.
Looks like you got it figured out Dave judging by your results.
I was successful as well.
I'm was using a 1/16 mill in Aluminum so I wasn't looking to go too fast, just a few ipm max. I like to take it easy.
I noticed that curves were not very smooth. I cut an "S" and it's pretty choppy. It could be I was taking too deep a cut (15thou)and the cutter was flexing. I'll have to try it again.
Your job with the word TAIG looks really nice Dave. What cutter were you using and also depth and speed would be nice to know for reference.
I also created the text with Autocad and rotated it before sending it through wrapper so the text went across (around) the end of the bar instead of along the length. I'm not sure of the quality of Auocad text.
I also had to edit the G-code a bit to pick upthe tool between letters because Autocad had left them linked for some reason.
I also had to change the default feed rate and add a separate feedrate for plunges.
What did you use to create the text?
Sage
-
Hi Sage,
I actually used a 30 degree .005" tip engraving cutter from ONSRUD and went about 7 IPMs, but obviously that varied when the X axis cut across the straight parts. I only went .005" deep and I'm using VCarve Pro to draw out the text. I've given up on LazyCam as I just couldn't deal with the finicky-ness of it all. VCarve is quite possibly the best CAM software I've tried and can't praise it enough, and the support over there is amazing as well.
Dave
-
Hi Sage,
Thanks for starting this topic, I'm sorry for jumping in and walking all over
your conversations, I re-read all the posts and I was Rude!!
I was just very Excited with the interesting 4th axis talk, so I just shot before I
thought. My apologies friend. (by the way, I use vcarve pro also, it really is that good!)
RC,
Thanks man ;) There are no shortcuts. Understood.
Very good subject and information gentlemen!
Glenn
-
Hey no problem. I got my answer and I thought we were all done. The diversion to a new topic resulted in more information for all. That's always good.
Sage