Fadal sudden circle problem

[PetePO]

Hello

Recently i've running long program containing almost only 3d waterlines on fadal . In my mastercam visualization there were no miastakes , normal 3d paths . In discriminator also everything was good. When i run it on fadal in the middle of path the mill suddenly went from 3d waterline to contouring some large cricle then went back to 3d path. My stepdown was 0.1 mm. Tolerance of path set to 0.025. What can cause these type of problem ?  

[#Rekd™]

Could be your minimum arc radius in the control definition. That can create issues with older controls.

[Colin Gilchrist]

Here are some possible explanations:

- You have an arc where the Arc Start Point and/or the Arc Endpoint, do not fall precisely on a Machine Grid Point.

- You have an arc where the Arc Sweep is very small, so the machine attempts to machine a full-circle.

- Same as above, small Arc Sweep, and the control interprets the move as "reversed" from what it really should be.

 

First, if you are using Radius Formatting, dump that in favor of IJK. The control has an easier time interpreting the intent with IJK.

Next, do you have the Control Definition set to 'break arcs at the quadrants"? < This option can cause "small arc slivers", for example; if you have an arc with 90.081 degrees of sweep, the CD will break it into a 90 degree arc, and a 0.081 degree arc. The solution here is to set the option to break at 180 degrees, or set "do not break", and enable the "allow 360 arc" checkbox.

Also, what are you using for Tolerance Values? What are your Arc/Line Filter Tolerance values?

Have you attempted to measure your actual geometry? I will always crank up my Analyze Tolerances to 2-3 decimal places more accurate, than my machine output. So if you are working in Inch mode, and your machine has a resolution of 0.0001, I would recommend measuring your geometry with a resolution of 0.000001. That allows you to see how Rounding could be affecting your Toolpath. 

If you have an Arc at X1.000041 and Y1.000032, and you have Analyze set to 4 decimal places, that Arc looks like X1. Y1., but mathematically; it is off by 41 Millionths in X, and 32 Millionths in Y. When you try to contour that Arc, those errors can be magnified, since you are making a radial offset for the centerline of the cutter.

 

[Thad]

I've seen this happen a few times on our Fadals. I believe (It's been MANY years) we narrowed it down to using R for radius instead of IJK. We switched to IJK and never saw it again.

[tryon]

Yeah I bet you had a R command with a digit before the decimal, like R1.25.  the fadal uses R values as variables so sometimes a radius of R1.25 would be read by the control as R1=.25.  Either format in a "+" after any R word(R+1.25) or better yet use IJK.   

[rickt]

#Rekd may have it.  The max radius in the Fadal is 399.9999.  Does strange things if that is exceeded.  There used to be a place in the post to limit this number but maybe that is done in the control definition now.  I also agree in using IJK.

Rick

[cncappsjames]

FADAL is synonymous with controls doing their own thing from time to time with no rhyme or apparent reason.

BITD, I was running one and the X axis just ran away on me. I almost got fired for it because "CNC's only do what you tell 'em to do" according to my then boss. Yeah,... until it ran away on him too later that day. The xxxx never even apologized. 

[PAnderson]

Colin is correct in his description. This isn't just something that happens on Fadals. Fanucs exhibit this behavior also. I had this happen twice on very expensive mold cores. And more recently, a customer was blaming the machine. While it was the machine in a way, the real culprit was the fact that tiny arcs were being created. If the end point is so close to the start point that the control understands it as a complete arc. In the case of our customer, the arc length was only .0002" with a radius of over 100". Somewhere in the CAM system, there needs to be a minimum arc LENGTH setting. Something the control does NOT see as ambiguous.

[Colin Gilchrist]

On 3/8/2021 at 8:21 AM, PAnderson said:

Colin is correct in his description. This isn't just something that happens on Fadals. Fanucs exhibit this behavior also. I had this happen twice on very expensive mold cores. And more recently, a customer was blaming the machine. While it was the machine in a way, the real culprit was the fact that tiny arcs were being created. If the end point is so close to the start point that the control understands it as a complete arc. In the case of our customer, the arc length was only .0002" with a radius of over 100". Somewhere in the CAM system, there needs to be a minimum arc LENGTH setting. Something the control does NOT see as ambiguous.

There are 3 places in Mastercam were we can enter tolerance data for creating "arcs" in a Toolpath. (Technically, there are 4, if you include the "Base geometry" as the first place where a tolerance comes into play.)

1. System Configuration Tolerance Page - Here we set a "minimum arc length" tolerance. This should generally be the smallest arc that you want to allow the system to create, in any of the toolpaths you are going to use. Min/Max Curve Step Size: These are the min/max step distances you want a toolpath to be able to use. I generally set my "min" value to 0.00005 Inches, and my Max value to 40. Finally, Chordal step size is typically 0.0004" for me.
2. Control Definition Tolerance Page - These are "global" values for Arcs, based on the particular machine you are programming. Here we have 4 values which come into play. The important thing to understand here is this > The default behavior of the system is to always "Break an arc into lines", if the parameters fall outside the min/max values we set in the CD. First Tolerance to come into play is the Minimum Distance between Arc Endpoints. Set this between 0.001-0.01". I typically use 0.002" for this setting. 2nd Tolerance is Minimum Arc Length. This is the circumferential distance. I like to use 0.0016" for this value. 3rd is the Minimum Arc Radius. For that value, I like to use 0.001". (Note: there is a relationship between a 90 degree arc sweep, and the circumferential length, of about 1:1.5 ratio. So if your Min Arc Rad was = 0.005, set your Min Arc Length = 0.0075". You do not have to maintain a ratio here, but you should understand how either of those "min" values can end up limiting the arcs which are created in your path.) Finally, the 4th Tolerance is "Max Arc Radius". I like to use 80" as my max arc radius, unless I know that I've got a true "circular section" to machine which is a partial arc, that happens to fit within the travel limits of my machine.
3. Tolerance > Line/Arc Filter Settings - This is where the rubber really meets the road, and we can set tolerances for a specific tool path that is being created. Here we can apply different "min/max" arc values, which comes in very handy for limiting those pesky "small arc radius or segment issues". Typically for a Roughing Path, I limit my "minimum arc size" to 0.020" and my "max arc size" to one of these values: (4", 8", 20", 40", or 80"). Generally speaking, we want all the small arcs, and medium arcs, to be output as an arc. However, we want "tiny" arcs, and "small slivers" of arcs, to be linearized.