Strange circle behavior, 151B control

[swarf_rat]

This is the sequence:

179 L X4.187 Y-0.969 R0 F48
180 CC X3.989 Y-0.936
181 C X4.189 Y-0.936 DR+ R0 F48

Causes an error "Circle Data Incorrect". Changing the X coordinate in line 181 to 4.190 fixes it. Whole bunch of these in the program, up until then all is well, after that, every one seems to error. Can't see why.

Any ideas?

[HuFlungDung]

It is most likely a rounding error, or perhaps two of them, in opposite directions creating a gap in the chain of endpoints that the controller does not like.

It may work better if you try using IJ arc center coordinates instead of R. If you have to tweak something, its better to tweak the arc center (to make the controller accept it) than it would be to change the endpoint of the move.

[gus]

Not familiar with that particular error, usually would expect 'circle end position incorrect' which is a little more obvious. If all of the circles are the same size try reprogramming them in incremental, labeling it and calling the label.

[swarf_rat]

Gus, it was "circle data incorrect". Rick at Heidenhain (and HFD) correctly identified it as a rounding error. Apparently the early TNC controls require that the circle math be exactly correct to 4 decimal places. The post was set up for only 3 places, rounding to that. Since in a C move the beginning & end point and center are defined, everything must match exactly. I guess I was luck on the first 50 or so moves, then hit the problems.

Now the problem I will run into is that the dwell time in a pecking cycle is only allowed to be defined to 3 places, and OneCNC only has one choice of places for all coordinates, so it is going to mess up my pecking cycles.

[gus]

PITA, but you can edit it in a word processor and find and replace the extra zeros

[HuFlungDung]

I don't think you'll see 4 place decimals in OneCNC for dwell, but that may depend on your choice of settings. I normally use 4 decimal places, but I get what I type in for dwell. What are you seeing happen?

[gus]

>>>and HFD<<<

wuts HFD?

[awemawson]

Originally Posted by gus >>>and HFD<<< wuts HFD?

HuFlungDung

[swarf_rat]

Originally Posted by HuFlungDung I don't think you'll see 4 place decimals in OneCNC for dwell, but that may depend on your choice of settings. I normally use 4 decimal places, but I get what I type in for dwell. What are you seeing happen?

I am using the variable DWELL. In the machine cycle dialog I type in "1" and I get "1.0000" if it is set to 4 decimal places. The control quits loading the program at that line, because (as Heidenhain Chicago confirms) dwell can only have 3 decimal places in this control. Is there some other parameter or variable to use that would produce only what I type?

I sure with the OneCNC folks would document their product. It would make it a lot easier to use, at least for me.

[gus]

I wonder if the software might have a parameter for removing trailing zeros

[HuFlungDung]

Swarf
Do you have to have trailing zeros turned on in your post?

There is another trick which we use to eliminate decimals from some numbers (like dwell, or repeats in a cycle) and that is to enter the number and a space to the number, this prevents a decimal from being inserted. However, I don't think this is your problem.

There are a lot of permutations of settings to make in nc setup, but the above mentioned 'trailing zeros' is the only reason I can think why you would be getting 4 zeros behind your dwell. I get the decimal, and that is all. Other numeric coordinates come in in 4 decimals as required.

[swarf_rat]

Hu,

You were right, turning off trailing zeros fixed that problem. But there may be related problems - however I will post those over on the OneCNC forum, since they are not of interest to any but OneCNC users.