Feeds and speeds

[svrfsvp@netscape.net]

I am just getting started with my ShopBot, and have encountered a problem cutting circles in 3/4" thick plywood - I am using a 1/4" diameter bit, the circle command reads as follows:
CC, 24,O,-1,0,0,-.25,3,1,1,1,1,1
which should do 3 repetitions, each 1/4" deeper than the last.

The problem I have is that the tool inevitably starts to cut a spiral towards the inside the circle rather than repeat the previous circular cut. Does anyone have any thoughts on what causes that to happen? I have some guesses, but it would be nice to have some concrete suggestions on how to eliminate this problem.

Regards...

[giggalo]

What I do and to me the easy way is in your cad program draw 3 circles with 3 diffrent colors and overlap the 3, then when you convert them it will ask for color depth the 1st would be -.25 the next color -.50 and the 3rd --.75 this will do 3 passes and cut thru all the way.

Make sure you remember what colors you did 1st 2nd and 3rd to enter the depth or you will go from -.25 to -.75, there might be a better way to do it but I always do it this way.

Ron

[stecchino]

Thanks for the input. I am using the ShopBot commands directly, and in programs that I have written, to cut some repetitive shapes - in this case, nested circles. The tool is going through the correct number of passes - no problem there, but what is happening, is that by the second or third pass, it starts to cut a spiral - that is, it fails to follow the path it used in a previous pass, and wanders in towards the middle of the circle.

What I am trying to figure out is what is responsible for this - is the controller dropping or mistranslating steps? Is the 1"/sec speed too fast, thereby overstressing the stepper motors? Is a 1/4" too much to cut in one pass? I am going through a lot of scrap in an effort to sort this out, and it would be nice to have some idea of what needs to be done to make the machine cut the same circle 3 times in succession.

[robin]

I use CC in the same way (i.e. 3 passes, 1/4" plunge per pass, etc) without problem so I don't think it is the software. I'm using version 2b8.

[stecchino]

Thanks - that is good feedback. What cutting speed do you use? I have mine set at 1"/sec., and am thinking that perhaps that is too fast.

[robin]

Speed? Depends. I tend to run things a little slower for circles, even .5 to .75, but watch out for burning. Moving your router (bit) too slow can cause your wood to overheat and turn brown, especially if your bit isn't sharp. In the early days I would often forget to adjust the speed for circle cuts. At 2-3 ips the router would rarely do 90 degrees of the circle before veering off.

That said, I would think 1 ips would be fine. After the cut, does the machine return to your 0,0 point correctly?

[Ted Hall, ShopBot]

Hi Jay,

It should work as you want. I can't make the simulator that I have with me fail ... but I'll try it on a tool tomorrow.

Might want to make sure you are in Absolute Mode when the circle starts (relative should work, but ...). Does the problem happen in a file, from the keyboard, or both?

I assume you're using Version 2 software, some of the extended functions are not in version 1.8.

[svrfsvp]

I tried to post a response last evening, I don't see it here, so here is another attempt...

Here are details of the circle cutting routine, which I tried again last evening, and which still results in the bit veering off course:

I have not tried this specific command using the keyboard, only from within the routine I wrote (see below for details),

Cutting speed is set at .5"/sec. in x and y,

Burning does occur,

Software version is 2b8,

Absolute mode is set before the cutting starts,

I checked the depth of the cuts, and the first pass was .375 instead of .25, and the second, which started to go off track, was .64, rather than .5, which makes me suspect the z-axis calibration, any hints on how best to do that?

The bit I am using is new, but I am going to get a spiral cutting bit and try that.

The routine I wrote follows:

'This program cuts a succession of circles, each smaller than
'the preceeding circle, the difference in diameter is set by
'adding the diameter of the bit and the desired wall thickness
'of the resulting ring.
SA,
SC,1
INPUT "Enter the bit diameter - " &bitd
INPUT "Enter the wall thickness - " &wthk
INPUT "Enter the diameter of first circle - " &dcir
INPUT "Enter the smallest circle diameter - " &smdia
&count=0
&diff=&wthk+&bitd 'add the wall thickness and bit diameter
'to calculate the starting point of succeeding circles.
&xspotone=&dcir/2
&yspotone=&dcir 'set x and y locations of first circle starting point
JZ, .5
J2, &xspotone, &yspotone 'move to 0 degrees of the first circle
MZ, 0
CC, &dcir,o,-1,0,0,-.25,3,1,1,1,1,1
&count=&count+1

circlecycle:
SR,
JY, -&diff 'change y location
&diar=2*&count*&diff
&cutdia=&dcir-&diar
IF &cutdia<&smdia THEN GOTO finish
SA,
CC, &cutdia,o,-1,0,0,-.25,3,1,1,1,1,1
JZ, .5
&count=&count+1
GOTO circlecycle

finish:
JH,
END

[svrfsvp]

Oh yeah, I forgot to mention - when the machine goes off track and I interrupt the command, when I do a JH command, it does not return to the original 0,0,0 location, but is off in x and y. Hope that provides another clue.

[Ron B]

Jay,

If it is a cable machine I'll bet cable tension is not right.

Ron

[svrfsvp]

I appreciate the info - but the machine in question is a rack and pinion machine, so it must be something else going awry - and I must say, I am stumped - just can't get it to cut circles. Perhaps the new bit, when it arrives, will change the outcome...

[phil]

Have you tried just cutting AIR without the bit cutting in the material. Your program is OK because it worked on mine.

Did you check it out on preview first? Is it OK in preview but fouls up when cutting?

I suspect a parameter problem.

[svrfsvp]

Yep, I have both run the program in preview mode and on the machine, cutting air. The problem arises when the bit starts cutting the plywood. Is there a specific parameter that seems to be a problem? I will gladly change any or all of them if the result is a working ShopBot...

[robin]

My guess is it's the bit. Either that or one or both of your motors/drivers is not up to specifications.

I should have added previously that if your wood starts to burn you should stop the cut since this is also very hard on your bits. Overheating is the quickest way to dull router bits (carbide is more heat resistant than steel). I always clean my bits whenever they start to show buildup. Let them sit in lye (old fashioned "full fume" oven cleaner) for anywhere from a few minutes to an hour, rinse them, then use a cloth to wipe away any of the softened residue still there.

[phil]

Ok, so the problem is only when the bit is in the wood. That would indicate a mechanical problem and not software or parameter setting.

What kind of bit are you using, straight flute, up spiral, down spiral?

I assume that you are using a standard clockwise turning router, did you try reversing the direction of cut of the circles to see if you get any change in performance?

You may also want to try shallower cuts and determine at what point the problem shows up.

If you bit is burnt from previous runs, you will definitely have a dull bit and that would compound the problem.

[svrfsvp]

Well, the mystery is solved - Ted Hall was able to figure out the cause of my circles becoming spirals, and boy is my face red! The bit, even though a single flute bit, was not the problem - it could cut all the way through the 3/4 plywood in one pass. The software was not the problem, even the command file I put together was not the problem, although I did rewrite it, on Ted's advice, to cut the innermost circle first, then work its way out. The assembly and setup of the machine was not the problem, it was within spec and producing enough power. Nope, it was none of those, it was in fact something much more mundane - and something that never entered my mind as a possibility - even though the work piece was clamped down, it was not clamped down well enough to prevent it from moving as the bit moved through the wood - thereby making the circles become spirals. The point where the bit entered to start the circle was not in the same place by the time the bit made it through 360 degrees. To quote Homer Simpson "D'OH!

In any case, my 'Bot is now cutting circles like a champ - fast, accurately, all the way through the plywood in one pass - what can I say - it rocks!

[sheldon@dingwallguitars.com]

I thought I read a thread about this elsewhere but couldn't find it.

How accurate are the move and jog rates? When timing a 40" move or jog on the x (I checked actual movement and it moves exactly 40")actual move and jog rates are approximately 60% of stated rates. Jog rate tops out at 2.5 ips.

[Gerald D]

Sheldon,

Try this topic:

Techniques for Cutting, Drilling, Machining: Run Time

[sheldon@dingwallguitars.com]

That was the thread I was thinking about, but after reading it, it didn't satisfy my question.

Of the people that have actually timed their jogs and moves, how accurate is the stated rate on screen compared to the actual measured rate.

Both my jogs and moves are at only 60% of what I've set them at. The distance moved is accurate, just the time it takes to get there is too slow.

[Gerald D]

Sheldon,

The published speed limits for the PRT model on the website today are:
x & y axis move 1.67 ips
x & y axis jog 4.17 ips

The age of your specific model could determine a different set of specs. We have seen a few different motor/gearbox/cable/rack combinations.

The PC that you supply may prevent the speeds from being achieved. This is discussed in the above-mentioned topic.

Yes, your observation is correct: the actual speed does top out, although the screen is displaying a higher value. Should we ask ShopBot for a "true" speed display?

[sheldon@dingwallguitars.com]

I swapped PCs and now my machine is performing beautifully.

On timed drag-race style runs, both move and jog speeds are accurate and in agreement with indicated settings. In this "unreal" environment, I am getting timed jog speeds of up to 5.25" per minute without missed steps. (I'll be dialing it down for real world use).

FYI the old computer was a Compaq non-Intel 180 MHZ and the new computer is an Acer P200.

[wecarve353@aol.com]

We are creating ncd files in casmate, then converting them in shopbot. For some reason, the created files have a jog speed of .333 for x & y. Our jog value setting is "2". This makes our files run way too slow. On small files, I can manually change the .333 to 2, but larger files are beyond me. Why are our files being created with the .333 setting? Our jog works fine, so it shouldn't be a motor problem.

[rgengrave@aol.com]

Bridget in the program you are using to make the ncd files you should see a display box for the settings when you select a driver.

If you are using Fanuc 2d or 3d driver? you will have to set the cut speed there.

You should see something like XY Speed Up or Down, by default it might be set to 20 inch? set this to 1 or 2 and this will correct the problem?

Now you might see Z lift and Z depth? you will want to make the settings in the Z lift if your Z is raising to slow, and the Z depth should be set to the depth you want.

Ron V

[Bridget Albano]

Ron, you were right. We raised the xy speed to 120 and got a decent jog speed. Thank you!