Choppy cutting

[Gary u]

I made a quick sign last night and I had a problem cutting out the oval.
I have noticed that cutting curves are somtimes very choppy. I read in a post some place that if the sharp corner box what checked then it will sometimes cause this to happen so I was careful not to select the box.

Here is the interesting part. In this sign I first cut the oval with a round over bit then I finished cutting the part al the way through with a 3/8 spiral bit.
It was the last profile cut with the 3/8 bit that was very choppy almost all the way around the sign. The pass with the round over bit was perfect.

Both bits are new.

The only differance between the round over bit pass and the spiral bit pass is that I had an offset allowance for the spiral.
At least this sign was made from MDF so I could sand out the marks but I need to find out what is happening.

The depth of cut was just over 1/2" and the speed was 450 ipm. The spindle speed was 18000 RPM.
(Should cut through this like butter)

I have noticed these kinds of things happening when I cut curves and I was using the shopsabre ATC Arcs Post Processor.

I have not said anything in the past becouse I was waiting for the new version hoping that some of this may be addressed.

If anyone has any ideas that would be a big help.

[RoutnAbout]

Gary,
Would it be possible to attach a picture of the edges of the actual oval sign you cut out?, Possible a close up of the edge. I know it my sound odd, but some times even new tools are not manufactured correctly ( I'm not saying this is the problem - but could be ) and I possible might be able to see if its the tool. How far apart or the choppy marks? Are the vertical on face of the side or are they at an angle on face of the side?

[Gary u]

I have already sanded the marks out, Stained the sign and shipped it.

But here is some additional information that might be useful.

THe marks looked like the oval was cut as a series of very short lines. Also, the cutting speed was a very slow crawl. It did seem to me when I was watching this happen that the cutter was cutting a series of strait lines say 1/4" long. This might be why the cutting speed was so slow and the choopy cuts etc.

As mentioned before, Cutting the oval with the round over pass was good and very fast. The differance was the offset I used with the 3/8 bit.

When I have time I will experiment with some scrap. I will take the file and cut the same oval with and without the offset to see what happens.

I will not have time to play with it until maybe Sunday.


Thanks

Gary

[TReischl]

Hi Gary,

What you don't tell us is how you created the oval? I am gonna try to keep this short and as untechnical as I can.

A machine control has a loop cycle time. Think of it like this, the machine sends out a command to move the axis a distance, then it takes a look to see if E-Stop was hit, then it looks to see if the software limits are exceeded, then it updates the screen, etc, etc, etc. This is know as the control cycle loop and is usually measured in milliseconds. In other words, your control only does one thing at a time then moves on to the next.

So, if your moves are very short, and your feedrate is nice and speedy, what can happen is that the tool reaches the commanded distance, but the control is not ready to send the next movement commands. So, the tool sits there. This can leave what appear to be small flats (especially if the cutter is a decent diameter, say a half inch).

Or, it could simply be that the program you used to create the oval actually did create tiny line segments, which can cause the above to happen, in addition to really making flats.

When I cut stuff that positively has to be great, I make sure I get rid of small movements by creating larger arcs through the points.

This is NOT a limitation of VCarve or your machine. I can make this happen on a half million dollar Mitsubishi laser by programming short line segments (in a straight live even) and then commanding a high feed rate. At first the machine moves right along, then the look ahead buffer empties out and you can watch that $.5 M dollar machine stutter. Which is what you called choppy.

Hope this has helped somewhat.

[TReischl]

I went ahead and took a look at your file and saved the outer profile path. Sure enough, you have straight line moves that are about .1 long.

First off, straight lines are going to leave flats, for sure. You did not need me to tell you that.

Secondly, the oval is quite large, around 26 inches, so there are tons of those short moves. You may have emptied the look ahead buffer as I mentioned in the earlier post and that would definitely aggravate the problem.

And, we might want to ask Tony and Brian if they could output arcs instead of short straight moves? Which could be a serious undertaking on their part.

Myself, I would draw that ellipse using a CAD package and using arcs to draw it. If you check, you will see that if you import arcs into VCarve, you get arcs back out.

[Gary u]

Thanks for the reply. I created the Oval with V Carve itself. The only vectors that are imported is the picture of a guy working on a control surface.

I do understand your comments somewhat but If this was the case, Why would the first of the two profile cuts work fine keeping in mind that both profile cuts are following the same vector curve. (I may have answered this on my own as said below)

I do have to say that i did make a mistake in my feed rate information that I said before. I looked again at the file and it was set to 600IPM not 450ipm.

Although the machine will cut at 600ipm, maybe there is too much information sent on a curve like this and slowing the feed rate to 400 might be the answer.

This is a simple test and maybe this weekend I will be able to play with it. When I set out to do this cut I did mean to change the feed rate to 450 but it looks like I never did. The first profile was set to 400ipm and it cut fine.

With this in mind, Maybe what you are saying is the case here. I need to run the file at 400ipm and see if that changed helps it.

It was as you say stuttering so bad that I did not know if it would even complete the cut or just plain blow up.

Gary

[Gary u]

I have had trouble trying to ask some questions becouse I did not want to come across like a complete idiot.

Now "I don't care" if I come across that way.

I admit that I am green as green can be when it comes to this stuff so I will start to ask what might be stupid questions.

You say that I can generate a oval with a cad program that is made up of arcs instead of lines. I have been using Turbocad for about 10 years and to this day I do not know how to do that or if they are made up of lines or arcs. I just select the oval tool and make it a givin size.

In the beginning of December 2006, Tony sent me a new post processor (shopsabre atc arcs inch pp) He had the following comments to go with it.

"Remember this only outputs Arcs for 2D pocket and profile toolpaths that are created from geometry that consists of lines and arcs. Regions with Bezier spans will be output as usual line moves."

I have to admit that I did not have a clue what he was talking about here. (and still don't) At that point, this was a new PP for them. A sort time went by and Tony called me to follow up on the processor file. For the most part I cut cabinet parts that are just strait cuts so it seemed to be working fine.

Can this be related to the oval outputting line segments as you noted?

Again, with me being green to this, How can I tell how a curve is made up?

Gary

[Jonmilligan]

Hi, I had this problem, and I asked the same question on this forum(see page 4"jerky profiling"). I have also used Turbo cad since ver.3 and went thru the same problems with arcs & lines with choppy output, I found that if you don't join the outlines of the profile that you want to cut(do not "join polyline" just group) keeping all arc segments and lines separate, it seems to cut OK.
Hope this helps!
Regards
John Milligan

[TReischl]

You are not a complete idiot. Not even close to one.

You have zeroed in on the two elements that are probably causing what you see.

1) A feed rate that exceeds the machines capability to process the information fast enough.

Think of it this way, if your machine could process the data fast enough, you would not have seen any stuttering, but you might have still seen some flats.

2. You know that VCarve produces straight line moves when you draw an ellipse. Most people do not realize that ellipses and arcs are two very different animals. Arcs are true radii. An ellipse can either be made up of arcs, or straight lines. If the straight lines are small enough, you do not see them.

I do not use Turbo Cad, but I do have it. I just made an ellipse using it. It stores it as an ellipse type. VCArve reads it and assigns nodes to the segments. Tony and Brian could make it come in as arcs but they have chosen this method. No doubt they have a good reason for doing it this way. Since I wrote software for CNC machines for 25 years, I do NOT question another programmers methods.

But, what you CAN do is this, go ahead and draw the ellipse using the ellipse tool in Turbo Cad. . . then draw right over the top of it using the arc tool. You could probably make that ellipse into about 16 arcs total. Remember, you would only have to draw one quadrant of it, then mirror it across the axis three times. Then, when VCarve reads it, it will have 16 cuts to accomplish instead of hundreds. Also these cuts will use G2 or G3 which means they are cut as arcs, not line segments.

I use this technique quite a bit on art work, because of exactly the problems you mention. It is the nature of the beast, there are no free lunches in CNC.

Hope this is helping you out some. The day is gonna come when I need help, cause I have needed it before!

[Gary u]

Thanks for your help. I have learned a new lesson with all of this.

I exported the oval and looked at it in Turbocad. In node edit, there were hundreds of nodes. I assume that this makes up the line segments that you are talking about.
I created the same shape with the eliptical arc tool. Then selected that with the node edit and there were only two nodes.

If I understand what you are saying then I assume that the processor would only be working with two lines so to speak instead of hundreds and I would get a smoother
operations / cut.

If I have to create shapes this way instead of within V carve then so be it.

V Carve is still a great program and I am very much looking forward to seeing what is new in V4.

Cheers


Gary

[Markm]

Hello Gary
I have a shop sabre as well and I have learned that to get a good circle cut I have to be running under 200IPM. The wincnc seems to loose its buffer like they discussed. Jim told me that with the servos and the laser that they have run the machines up to 1200 ipm and not lost the buffer but I think that it slows after running a bit. You can do an arc test in the machine to make sure that the software is prossesing arcs correctly. If that has a scalloped look then your servos need to be adjusted. Or so Jim explained to me. I am still having a bit of an issue with arcs and curves however being choppy but just on 2 sides so if you devided a circle into quarters it wook be 6 to 9 and 12 to 3. I have to call then back again and see what he can do. It is a very well built machine but I am not sure that I like wincnc. It seems to me that when I was running Mach 3 on my homemade machine I could achieve almost as much speed and it had all the features and more of wincnc. If I had steppers on my machine I would try runing that and see how it compaired for speeds.

Mark M

[TReischl]

A symptom of too many commanded motions vursus the speed of the machine is that you will see part of an ellipse cut perfectly fine, then it suddenly goes bad. This is when the buffer has become depleted.

As a side note, if you see 'dings' at the four cardinal points of a circle, this is usually a sign of backlash.

It is also important to understand that a CNC machine does NOT move in a circular manner ever. Yup, that is right, all those circles are not round at all, but made up of tiny short line seqments. When a G2 or G3 is commanded, the control does an internal calculation for all the points it needs. These points are handled very differently than the way points on an ellipse are handled. That is why you do not see the buffer become empty on large circles. However, if you program a series of short arcs, you will see the same problem as you would see with an ellipse trying to be cut at too high a feed rate.

The only machines I know of that overcome this problem have controls built on parallel processing (two computers acting together) One of the computers only does the motion, the other handles all the other stuff, like watching for E-stops, limit switches etc. This method drastically reduces the loop cycle time of the control.

The other thing we all need to do is make sure the computers we are using have nothing running in the background. Handy little utilities, cutesy stuff, etc all takes up processing time. I like to think of it this way, if you had a guy running a Bridgeport mill, you wouldn't want him watching TV while he was doing it, cause sure enough, he would either be real slow, or mess up.