UCCNC Turn Problems

[andrej]

OK, thanks. Unfortunately there is no settings in the F360PP to output G7 I parameters any other way than they are by default. I assumed that they were generated automatically depending on other settings. Maybe it can be somehow modified in the PP, but it is good to know that UCCNC is working just fine .

So the default LCNC PP in F360 library is written incorrectly, or perhaps LCNC can recalculate G7 I parameters when the file is opened and G7 is specified. No idea to be honest. I only know it opens it without any problems...

But since the G8 works OK I am personally fine with that as I do not care whether the machine runs in G7 or G8. When I have some time I will look at the PP some more and try to find if it is possible to adjust the I parameter when in radius mode.

[cncdrive]

OK, I will change the I parameter to diameter mode when in G7, so then it will be compatible with the LCNC post processor.

I'm not sure if LCNC or UCCNC is incorrect, I will have to look this up, because G7 is not in the RS274NGC standards.
So, I'm not sure which method is standard, but probably the LCNC method is more logical, because I defined in increments, so radius/diameter change for that between G7/G8 is not that logical.
So, anyways, I will change the I parameter, so it will work with the LCNC post.

[andrej]

Great, let me know when the update is done, I'd be happy to test it.

[cncdrive]

OK, we plan to release 1.2117 soon and then you can test it.

[Joachim]

I corrected the G7, X is multiplied by 2, but arcs are not good, I need to be doubled also?


https://github.com/JoachimF/UCCNC-Lathe-HSM-PP

[andrej]

Yes, the "I" parameter as per previous comment from cncdrive.

[cncdrive]

If the "I" is multiplied by 2 then it looks like this:

All I did is I simply multiplied all the I parameters the g-code file with G7 which you uploaded here.

[cncdrive]

And no, you do not have to double the "X", you only have to double the "I" parameter.

[Joachim]

Hi cncdrive,

We will do a review about G7 and G8

In G8:

G0/G1 X = radius
G2/G3 X= radius i=? j=?
G76 X= radius i=? j=?

In G7
G0/G1 X = diameter
G2/G3 X= diameter i=? j=?
G76 X= diameter i=? j=?

For now I compare output between grbl ouput in g8 and linuxcnc output in g7

Correct and complete my table, tell me what uccnc need, i'll code it.
What about the tool table and offsets. A button Diameter or Radius should be nice.

[cncdrive]

Hi,

Only I parameter matters, because I parameter is the arc center point along the X axis.
The J or K parameter is the other axis, it is not the X, so it does not matter if it is programmed in G7 or G8.

I think the problem is only in G2/3 arcs with the I parameter only.
I modified the g-code file of Andrej with multiplying the I parameter by 2 and the code looks OK now.
So, if you can then try to adjust the post processor to change the I parameter to 2x in G7 mode.