Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Workinforwood on October 17, 2011, 12:29:50 PM
-
I am having issues figuring out how to control my speeds. I am using a Syil x5 speedmaster. I have an A axis running, and it's max speed is 23.5 inches per minute. I don't know what my other servo speeds are, I can only assume they are the same? My problem is that the x is moving far faster than the A. I don't mind the speed the A is running at. I'd like to bump it up some, but then the x will move even faster. The problem I have is only when X runs in a straight line. I'm cutting some letters right now, so take the letter M for example. The a will turn to put the bit in position. Then only the x needs move the straight line on each side of the m. It takes off like a rabbit and breaks the bit. When A and X move together, like the v inside the M, there is no issues, they move nice and easy. I want to bump up my speed, it's taking too long to cut the letters, and the bit is capable of more travel speed, but not the kind of speed it's running in x only mode. If I boost the speed, it boosts both a and x, so that's not good. I want to boost A and slow down x. I am not sure how to do this. I tried going into the motor tuning and dropping the speeds for x, but then i get a pwm error.
-
Your A axis should be set up for steps per degree if its a rotational axis.
Hood
-
ok, how do I do that? I did do the set up procedure to auto config the travel of the rotary table...it asked me how far to move it, so I say 20 degrees, then it moved it and asked how far it travelled and it was 15, so then it reset it and I did test again and it was good. Is this the same thing you are talking about?
-
I prefer to calculate rather than have Mach work it out as that way relies on your measuring.
Ok do you have the axis set up as a rotational axis on General Config page?
There is also an option on the settings page I think that allows you to enter the radius of the 4th axis work which you may need t set depending on your code. If the X flies away when it moves on its own then it would seem the feedrates in the code are the problem.
.
Hood
-
The x does not fly away, it just flies across the piece super fast. It is doing the correct cut path, just at sonic speed, the A is slow. When they work together, there's no problem, it's just when the x moves in a straight line without needing a that the speed jumps way up. The code does set the radius of the piece being cut. Everything is actually cutting perfect, it's just when that x axis has the opportunity to do a cut without combining with a then she speeds way up. When combined with A it's way slower than i'd like. I need to find the happy medium.
Maybe this will help. Here is my motor tuning settings
Steps Velocity Accel
x 10160 31.158 31.158
Y 10160 100.02 12
z 10160 129.42 50.5
a 400 1000 1000
My software Settings from Visual Mill 6 for cutting 3 letters on a tube, 4 axis pocket
Bit is 0.024
Plunge 25 in/min
Approach 25
Engage 22
cut 17
retract 25
depart 26
Total cut depth is .07
Finish Rough depth is .056 and finish depth is .014
Rough depth cuts are .0224 <but that's what it's supposed to be. The machine is cutting right now and each layer is not .0224, it's cutting layers at .0117 for whatever reason I don't know.
-
Your speeds in visual CAM are fast I would say and that is what the X will be running at when it is moving on its own, the reason its slower when in conjunction with A will likely be because A is a much slower axis (2.77 rpm approx) so X feedrate will be slowed down accordingly.
Hood
-
ok..what kind of speeds would you choose?
-
oh..also, is this the reason that the PWM error kicks on..I am asking the machine to move too fast?
-
I dont know what kind of speeds as it would depend on cutter size, amount of flutes, spindle speed capability and material being cut. I dont have a clue about wood so if thats what you are cutting someone else will hopefully answer.
PWM error is likely due to spindle speeds being set too high or the spindle not being set up correctly, afraid again I dont really know as I have only ever used servo spindles with step/dir
Hood
-
I am cutting plastic rod. I figured out the PWM issue. Right on the very last page, troubleshooting in my mill manual. I needed to change motor control. It was 500 and 15%, I needed to change it to 500 and 0%. Since then, no more PWM error. Things seem to be working much better now. I did not change any of my programming speeds. The tiny bit is cutting great at those speeds. I actually think it can handle more, but when I bump my speeds, the rotary table speed does not increase. I think it's just a slow table, does like 1000 degrees per minute..seems to me though that is faster than what it is doing. No doubt i'll get that worked out. Right now I have to figure out what's going on with my software. I'm cutting like a letter A and an M and both letters have a box at each corner. The boxes at the bottom of each letter is cutting out spot on perfect. The boxes at the top of each letter are cutting out perfect except for across the top of each box is not flat it is V shaped. It's strange. I had to do a manual clean up jog across the top of the two letters to clean them up.
-
TO have any speed on the A axis as a 3d type cut you need to sync to the A part diameter so MACH acan figure out the proper relationship of the X and A speeds to BLEND the move. Otherwise Mach picks the slowest combination it is aware of "the a axis speed". BUT as you have found IF you make a staight X move it runs at the actual speed called for.
Just a thought(;-) TP
-
Interesting. How do you sync to the A part diameter?
-
Go to gen config then toolpath config. Check the box for USe radius for feedrate.
THEN go to the settings page ,top right and insert the values of the A axis part as a radius.
That will allow MACH to know what the true surface speed of the part is based on the radius AND allow it to better blend the feedrates of the XY/A.
Just a thought(;-) TP
-
Sounds awesome, thank you. I am cutting right now, when finished I'll give that a try!
do you think that will fix this other problem maybe? This pic is for the Texas AM logo. I have a guy working on licensing and I am making his samples. In Visual Mill 6, I created this and in Simulation mode it works perfect. Each letter has a box on it, so like the A has 3 boxes, one on top and 2 on the bottom, that's just how they font their letters. I cut this out and the T is flawless. The A and the M are perfect but not on top. If you look close at the pic you can see the box on the top of the A. It should be flat across the top, but it is V shaped. The boxes on the bottom legs of the A are perfect. The M is doing the same thing. The 2 top boxes on the M is v shaped and the leg boxes at the bottom are perfectly square. It's bizarre. I sent my program to Visual mill and they say it's perfect, got to be some other issue. Right now, I am able to still make these samples, but what I have to do after it is cut is jog the bit with my mouse into the top square and carefully buzz across the top of each box to clean and square it up. It's not easy, but it works, and it sucks having to do it.
(http://i121.photobucket.com/albums/o202/workinforwood/LogoA.jpg)
-
MACH3 will only do as it is told to do(;-).
The only way to know for sure is to post the program and let someone else test it or at least let us reveiw the code to see IF we can spot anything that may cause it.
IF you do not wnat to publicly post it (not always a good idea with copywrite/trademark materials) then you can email it direct to me.
BUT before you do that try the fix it may just be a case that with CV turned on and a slow axis it created rounding arcs where a square corner should be.
(;-) TP
-
ok, thanks. I have something to try first and if it doesn't work out I can do that. I want to get these perfect as I can so the customer can get the legal rights to it. The visual mill guy gave me something new to try, some kinda edit in my posting process that might fix it. I have about an hour or so left on the current part in the machine. Then I'm going to do the mach edits and load in the new software edits and see what happens. Hopefully it will cut much faster this time too. The visual mill says it should take 7 minutes, but the real time it has been taking is 2 hrs 41 minutes. Be sweet if I could even just do one in an hour, then I could be profitable! I have a lot of money tied up in this machine. Good news is I paid cash. It's been a real struggle the least few months, but I feel much better every day using it. I actually drew this logo using the mouse and visual software, posted all the stuff, 100% accomplished it by myself this time! Every bug I encounter and fix teaches me a whole lot..I learn best by my mistakes. Heck..you see the tape on this rod..yea, I learned that fast, no tape and the rod can slip in the bushings and get trashed out by the bit. DAMHIKT..lol!
-
WOW>>>HAHAHAHA!!! You guys rock! Hood...you were absolutely correct about the speed was too fast. I about jumped out of my shorts when it took off after making the suggestions of the second kind sir! I cut this design, it took 2 hrs 40 minutes. Now I recut, took 4 min 48 seconds! Plastic dust was launching. I was about to do a manual over ride and slow it down but thought heck..let her go and away she went. She cut that baby out super sonic speed. It did break off a few pieces, but I actually don't think the speed was the issue, the rod was an extra one where the inside hole I accidentally bored a touch too big, so the depth of the hole ended up going all the way through the rod and that's why the center of the A disappeared and part of the inside of the M broke off. I will slow it down next time, but not hardly by much. I got the boxes on the top of the two letters perfect too.
This was the suggestion to try in the visual mill and it worked out.
Can you try setting the Co-ordinate output in the post to non-modal and see if this makes any difference?. To edit the post processor, select Set Post Options (2nd button on setup tab), Click edit next to current post processor. This opens up the post processor generator.
On the General tab, clear the check box for Co-ordinate under Modal Output. Save and close the post processor.
Now post process your toolpath.
Setting the co-ordinate to non-modal, outputs X Z and A co-ordinate motions for every line of code.