Need Help!- G2\G3 help

[soonervols]

After much searching and unable to find what I am looking for. I leave it in somebody elses hands.

First off I am running a HAAS HL-2 and Victor TNS-3 w/Fanuc 10T lathes. My main point is finding a very simple way of calculating I & K. I have found nothing that is clicking in my head to better understand.

Second, I have a part with two radius running into each other. A outside radius of 9/16" going into an inside 1/2" radius. I have it programmed using "R" but it leaves a step where the two radius meet. My thinking is using I & K will blend them together more smoothly. Is this a correct thinking?

The part is made from 2" round, length of part is 1.0935, Z will move a total of .7815. I am just looking for the final pass my tool will make. Using DMNG432 insert.

Thanks in advance for any and all help.

[sld4121]

Using I and K for G2 and G3 moves will always be more accurate and in some cases there is a potential of two different tool paths. Since I never like the machine to choose for me, I never use R values. Now the question becomes how good is your Trig?
In any case, it appears to be a simple request, so send me a copy of your print and I will punch a couple of numbers for you.
However, bear in mind that you are dealing with old machines, so you may find that you have more of a mecahnical issue than a programming issue.

[angelw]

Originally Posted by soonervols After much searching and unable to find what I am looking for. I leave it in somebody elses hands. First off I am running a HAAS HL-2 and Victor TNS-3 w/Fanuc 10T lathes. My main point is finding a very simple way of calculating I & K. I have found nothing that is clicking in my head to better understand. Second, I have a part with two radius running into each other. A outside radius of 9/16" going into an inside 1/2" radius. I have it programmed using "R" but it leaves a step where the two radius meet. My thinking is using I & K will blend them together more smoothly. Is this a correct thinking? The part is made from 2" round, length of part is 1.0935, Z will move a total of .7815. I am just looking for the final pass my tool will make. Using DMNG432 insert. Thanks in advance for any and all help.

In all cases, there will be some known features that can be gained from the part drawing or the previous tool location. Whether the arc involved is tangent to, or intersecting another line or circle, the I & K values can always be determined by using trig functions or Pythagorean Theorem.

Make a sketch of the arc detail and whatever element its tangent to or intersecting with, and draw in the Tool Nose Radius in its correct location relative to the two elements. Construct a triangle with the hypotenuse being equal to the arc plus the TNR and fill in any known values. From here its a relatively simple exercise in trigonometry to find the I & K.

The attached picture shows a simple example where, because two sides of the triangle are known, the side that will be the K value can be determined using Pythagorean Theorem.

Wit regards your other question, make a sketch of the part you want help with the code for and post it.

Best regards,

Bill

[camtd]

There is a nc editor called NcPlot it will convert R values which are easy to program to I, J or K's depending on your plane. The website is NCPlot.com - Tools for CNC Programmers

[angelw]

Originally Posted by camtd There is a nc editor called NcPlot it will convert R values which are easy to program to I, J or K's depending on your plane. The website is NCPlot.com - Tools for CNC Programmers

The thing is with programming using R in circular interpolation commands, is that if the end point is not correct, the control will shift the arc center to make it work. Now this may be OK if you just want a blend radius, but if its an accurate profile that you're after, then programming with R won't detect an error if your end point in not on the proposed arc trajectory based on a fixed arc center, it just shifts the arc center to make it fit. Accordingly, if your end point calculations is not correct, and R is used in the command line, then software to convert to I & K will calculate a best fit I & K, based not necessarily on where the center of the circle should be.

The mathematics for calculating the center of a circle given two points and a radius is quite straight forward, and something like the following would be used by the control, or software to calculate I J and K values from programs using R values.

For every two points and radius, there are two arc centers that will satisfy the arc passing through the two points with the given radius. That's why Fanuc, and probably other controls, use -R when the arc is greater than 180degs. Once the center coordinates are know, the I, J, or K values are easily obtained by comparing the center coordinates to those of the arc start point.

Regards,

Bill

In the following math:
r = the arc radius
X1,Y1 = the start point
X2,Y2 = the end point

If the arc is 180 deg, only Step 2 is required.


Step 1
Get distance between 1st and 2nd points
q = Sqr((X2 - X1) ^ 2 + (Y2 - Y1) ^ 2)

Step 2
Find mid point of q (X3,Y3)
X3 = (X1 + X2) / 2
Y3 = (Y1 + Y2) / 2

Step 3
Find center point of arc
X = X3 + Sqr(r ^ 2 - (q / 2) ^ 2) * (Y1 - Y2) / q
Y = Y3 + Sqr(r ^ 2 - (q / 2) ^ 2) * (X2 - X1) / q

X = X3 - Sqr(r ^ 2 - (q / 2) ^ 2) * (Y1 - Y2) / q
Y = Y3 - Sqr(r ^ 2 - (q / 2) ^ 2) * (X2 - X1) / q

[soonervols]

I will try to get the engineer to make me a copy of the print I can post tomorrow.

[soonervols]

Excuse my crude attempt at a drawing. Just in case someone didn't want to wait on actual print.

[sinha_nsit]

Originally Posted by soonervols ... Second, I have a part with two radius running into each other. A outside radius of 9/16" going into an inside 1/2" radius. I have it programmed using "R" but it leaves a step where the two radius meet. My thinking is using I & K will blend them together more smoothly. Is this a correct thinking? ...

Make an accurate scaled drawing. If you see a kink in the drawing, it would appear after machining also. Center method, or any other method, does not "blend" the arcs. However, center method has to be used for 180 deg arcs. Radius method is not accurate for half circles.

[angelw]

Originally Posted by soonervols Excuse my crude attempt at a drawing. Just in case someone didn't want to wait on actual print.

Quite a few assumptions here, as there is not enough information on the sketch to do any calcs without some assumptions:
1. The X center of the 1/2 rad circle is on the 0.312" line
2. That the 0.312 line is at diameter 2.0"

Given the above, all of the coordinates to create a tool path can be calculated using trig. In all of these manual calculations, it helps to sketch in the triangles relative to the points you need to obtain.

The green circle represents the TNR of your tool, and once Angle A is obtained, all dimensions of any other triangle can be obtained if the dimension of one side only is known. In this case the hypotenuse of two of the triangles are the radii of the respective arcs. The hypotenuse for the triangle required to obtain the center of the TRN is the 9/16" radius + the TNR when calculating for the I and K for it, and 1/2" radius - TNR when doing the calcs for its I and K values. You need to do it this way if not using cutter rad comp (G42), as the true center of the TNR has to be calculated. If the X and Z edge of the TNR is used to set the coordinate system, then you can calculate these points for your program by applying TNR value to the calculated TNR center coordinates.

You should make a drawing closer to scale than the sketch you've posted. Your sketch shows two radii that are quite dissimilar, yet in fact they only vary by 1/16". The attached picture shows a correctly scaled drawing, but is based on the 1/2" radius having its center on the X2" diameter line, and the 9/16" radius being tangent with the 1/2" radius and the face of the work, ie, Z Zero. The scale doesn't have to be perfect, just reasonable so you can better visualize the part.

If your quest is to learn how to calculate a tool path manually, then the attached picture will give you some insight in how to go about it. Alternatively, if you're only interested in the resulting program, post a sketch with a bit more detail and I'll send you an accurate tool path.

Regards,

Bill

[soonervols]

Ok fellas here you go. Thanks for all the input so far.

[angelw]

Originally Posted by soonervols Ok fellas here you go. Thanks for all the input so far.

Finish tool path.

Regards,

Bill



(0.031 T/N RADIUS)
G00 X2.188 Z0.169
G00 X0.338
G01 Z0.000 F0.050
G01 X-0.062 F0.008
G03 X1.081 Z-0.436 I0.000 K-0.593
G02 X1.841 Z-0.774 I0.452 K0.125
G03 X2.000 Z-0.867 I-0.015 K-0.093
G01 X2.188 F0.050
G00 Z0.169

[soonervols]

Thanks Bill,

That worked great. Now if I just understood how you did that or how you got your I & K numbers, I would be in business. The only trig I know is what has been self taught over the years. So no real understanding of it, lol.