Mind offically blown

[ahaslam]

I just spent a few hours learning something about my machines I never knew. I posted out some code, no problems. I intended for it to cut a bore that was 7.285 in Dia. Ran the code fine but it cut the bore 7.260. checked my numbers, then checked my numbers again. Nothing was wrong with Mastercam. Then I checked the code. We use R values, not IJK. Did the math on my R value. That was good. So everything seemed fine. We tried a few things but nothing would work aside from comp-ing the tool out .025". We had some down time to mess with it and we figured it out. I just don't know why. My boss came in and said why not try changing the geometry from 7.285 to 7.284. I gave him a dumb look but hey, he is the boss. I tried it and sure enough. It cut a 7.284 Dia bore. He said bores sometimes have to be an even number. . . I doubt that. I think what is going on is my start points for my R value are not posting correctly or something. Any one feel like reading over the code and seeing if they see what I am missing?

 

Code that fails to cut a 7.285 (cuts it to 7.260) Dia bore using Contour with a .75 end mill

 

X-.225 Y-2.6675
G41 D34 Y-3.0425
G3 X0. Y-3.2675 R.225
Y3.2675 R3.268
Y-3.2675 R3.268
G1 X.01
G3 X.2343 Y-3.0418 R.225
G1 G40 X.2332 Y-2.6668

 

Code that cuts a 7.284 Dia bore using Contour with a .75 endmill

 

X-.225 Y-2.667
G41 D34 Y-3.042
G3 X0. Y-3.267 R.225
Y3.267 R3.267
Y-3.267 R3.267
G1 X.01
G3 X.2343 Y-3.0413 R.225
G1 G40 X.2332 Y-2.6663

 

 

 

 

 

 

[TheePres]

I can't offer suggestions on why, but out of habit I have always also done as your boss and changed bores to even number.

[TheePres]

I can't offer suggestions on why, but out of habit I have always also done as your boss and changed bores to even number.

[gcode]

Try changing to IJK

I have been burned many times using R

[The Cathedral]

I'd be more concerned about the fact that your R values are incorrect. You need a 4 place output, yours only have three and thus the numbers don't add up.

 

(3.268*2)+.75 = 7.286

 

It doesn't account for the huge difference in diameters, but it explains why he wants even numbers: to eliminate that extra .0005

 

Your post is truncating it, and that probably leads to compounding errors.

[ahaslam]

Theepres, are you having this problem as well? Do you always change it to an even number? 

 

 

Gcode, I preffer IJK, but I am not the one running the machines and majority vote has been keep the R values.

 

Cathedral Yeah, I changed it to a 3 place decimal by request of the machinist on the floor. I quote "using a 4 place decimal point in your R value will cause these machines to make holes out of round".

 

Edit, side note, I have never tested the out of round problem.

[Thad]

Gcode, I preffer IJK, but I am not the one running the machines and majority vote has been keep the R values.

 

Cathedral Yeah, I changed it to a 3 place decimal by request of the machinist on the floor. I quote "using a 4 place decimal point in your R value will cause these machines to make holes out of round".

 

 

I think I see where the problem is.

[ahaslam]

I think I see where the problem is.

 

Yeah, I don't have any back bone.

[guitar]

Theepres, are you having this problem as well? Do you always change it to an even number? 

 

 

Gcode, I preffer IJK, but I am not the one running the machines and majority vote has been keep the R values.

 

Cathedral Yeah, I changed it to a 3 place decimal by request of the machinist on the floor. I quote "using a 4 place decimal point in your R value will cause these machines to make holes out of round".

 

Edit, side note, I have never tested the out of round problem.

 

 

Keeping the R values is incorrect. The IJK values should be used. I have seen several issues where R values do not give you the correct shape; where as, IJK always does. Also, as Cathedral states, do not round off to 3 decimal points. Another thing, break your arcs into quadrants.

[The Cathedral]

Theepres, are you having this problem as well? Do you always change it to an even number? 

 

 

Gcode, I preffer IJK, but I am not the one running the machines and majority vote has been keep the R values.

 

Cathedral Yeah, I changed it to a 3 place decimal by request of the machinist on the floor. I quote "using a 4 place decimal point in your R value will cause these machines to make holes out of round".

 

Edit, side note, I have never tested the out of round problem.

 

What kind of machine is it? What control?

[gcode]

majority vote has been keep the R values

 

manufacturing is not a democracy

post the file out with IJK arcs and see if you get a good part

[Radical1]

break your arcs into quadrants.

 

Just wondering, won't this give you extra hesitation marks or gouges in your bore?

[jlw™]

I detest R values. IJK and you'll never see this again.

 

Why would an operator have a preference any way?

[Mick]

I back up what others have said here. Use IJK and don't use R.

 

Way way way (Way!) back I thought R was the way to go. But then I encountered the occasional problem with R, but never with IJK. Nowadays, I never use R.

[mkd]

Why would an operator have a preference any way?

might be a <possibly false> sense of mastery.

machinists think they know what the code is going to produce easier than IJK.

at least that was the case when i was finger camming 50 part cycles in the '90's.

 

 

this is a tough issue mostly solved by IJK broke into quadrants. more code=less interpretation error.

I've seen IJK gouges that R solved

[GIZMO 21]

same here. I used to use R's also, then started to have problems with holes and corner radius. i would run the original hole size (7.285) using ijk, and see what happens.

the worst that can happen is you're gonna cut a hole to size, cause now the hole is undersize using r values.

most of time preference is not up to the operator/machinist. it's what ever the machine likes.

[TheePres]

After switching to IJK I no longer have that problem. But I still,out of habit from being burned in past, round up to nice even numbers.

[mkd]

I can't offer suggestions on why, but out of habit I have always also done as your boss and changed bores to even number.

 

 

After switching to IJK I no longer have that problem. But I still,out of habit from being burned in past, round up to nice even numbers.

mind=blown

 

i've never heard that.

interesting.

[jlw™]

mind=blown

 

i've never heard that.

interesting.

I've never heard it either... but I've never had to punch tape to program!

[CJep]

 But I still,out of habit from being burned in past, round up to nice even numbers.

 

 

Then how would you accurately describe a tangency for a polar arc that does not start or end at the 90deg quadrants?

[djstedman]

Machines usually have a parameter that specifies the allowable "acceptable error" between endpoints when using a R value rather than an IJK and depending on how large a value is in the parameter you can get wildly different results on different machines, this is why IJK value will consistently create a better hole.

 

When you use an R value rather than an IJK value you are letting the machine calculate where the center of the arc is in relation to the endpoints, when you use IJK you are specifying the center point of the arc as well as the endpoints .. that's why you get a better result.

[ahaslam]

Thank you for all the replies. I didn't anticipate getting so much feed back. I am going to push the IJK thing the next time this problem comes up. It makes sense that the machine may be making minor errors in calculating the center point. This could be why we sometimes get holes that are out of round. The machinist here are good guys. They just have a way they have always done things and that's the way they want to do them. They about crapped the pants when I showed them dynamic machining. They ALL had something negative to say about it. Every thing from the code is to long (they do have a point with that, DNC sucks) to it's too hard on the machine. The fact that it cut machining time by more than 30% was of no concern to them (they live by the say "getting paid by the hour"). In the end it isn't up to me, it's up to the boss. He tends to side with the guys that have been here 20+ years. Non the less I don't want to see the shop falling behind because it is stuck in its old ways. Thanks again.

[ahaslam]

What kind of machine is it? What control?

 

It is a Matsuura with the Yasnac control

[taperlength]

the problem is the 3 place R values are larger than the X Y move.  That shifts the center of each arc.  If you measure the bore in the Y direction it is probably to size but smaller across the X direction.

[Mick]

I've never heard it either... but I've never had to punch tape to program!

 

I've done that! Actually, I still have two tape punches in my garage. Would you like some sample tape punched?