Possible bug?

Guys

I generated some code using DXFtoGcode and also in GCNCCAM (it does not matter which same result in the end), loaded it and run the the code and worked fine. generate more code for new objects and loaded it and EMC complains about gouging in concave corners. This happens no matter what generator i use and works again if i create a new machine profile (stepconf) then load the code and its fine until i load the next file. The code is good and all i can think of is that the tool compensation is being held in the config of EMC somewhere? The tool table only has one tool in it with the correct diameter of cutter (4.5mm). i've attached the code if you want to see and would appreciate any feedback please it's doing my head in.

ps

The code is just a guide and it does not matter which drawing i use created from any cam software (even mastercam).

The code loads for me with a 0.075" diameter tool but no larger. Do you know when you change the tool table you have to reload it?

John

Yes john i reload the table but makes no difference.

Does the code genuinely have radii that the tool can't touch?

I can't view the G-code other than as text here, but your first G2 move looks very tight for a 4.5mm tool.

The biggest tool you can use with your code is 1.9mm due to your path being too tight for anything bigger than that.

John

I sent the code to a friend to run on Mah3 and it run straight out the box. I'm still confused why it would work fine if i create a new machine profile, it loads straight up and runs without a quibble? Should i be looking at any config files in EMC to see if any change before and after in the scenario i describe? Do machine offsets get written anywhere and not clear properly afterwards? Both the code generators produce similar code and the same thing happens regardless. John you said the code loads fine on yours? T1 is set to 4.5mm in the tool table so still not sure the code can be at fault here. It will have to wait till tomorrow but i will set some smaller bits to see what happens. Just to note the drawing does no appear when i load the code just a small dit in the middle of the table (roughly where start position should be). Thanks for the feedback so far
Paul

2e0poz wrote:

T1 is set to 4.5mm in the tool table so still not sure the code can be at fault here.

But it is wrong.

Your first G2 move demands a 3.182mm diameter hole with diameter compensation active and a 4.5mm dia cutter.
(G2 is clockwise, G42 is cutter to the right)
That is simply not possible, and EMC2 points that out to you.

You say that the code runs fine in Mach, but I rather suspect that after that first move there isn't a 3.182mm diameter hole, there will be either a 4.5mm hole, or possibly a 5.818mm dia hole. The difference is not that Mach is superior to EMC2, but that it doesn't have gouging detection.

If you are trying to leave a 3.182mm dia "peg" then you need to either make the first cut a G3, or use G41 compensation.

2e0poz wrote:

Just to note the drawing does no appear when i load the code just a small dit in the middle of the table (roughly where start position should be). Thanks for the feedback so far
Paul

Only that portion of g code that is runnable (no errors in coding) will display on the back plot. As soon as the error is discovered then the preview stops loading at that point and does not try and load any more. As Andy pointed out your code may run on other systems without gouge protection but you will not like the part when it is done.

John

Guys

i think i understand now and can see i will be a while in getting to grips. As for Mach being more superior that i feel not, i do like the sound of the protection i am actually getting from EMC. I will have a play with the tools today and would like to thank you for clearing this up. This is what makes EMC a great community and not just a tool.

Many thanks

Paul