Avoid Post Conversion Problems / Crash with testing.

[carbuthn]

I am putting this in a new thread because the problems are not part of the conversion process, but more about testing issues that could apply to anyone.

The lathe is like the Centroid test lathe (Isle Techno, ClearPath drives, encoder, and GS2 VFD (pictures are in Yet Another Techno Lathe thread).

Performed calibration of the Axises. All within 0.001 per inch of travel (X is per 1/2" of travel for 1" demanded travel). Set the tool offsets for 9 tools. Picked the Pawn to start testing with. Edited the file to use tool 2 (55° right as used in the video) and 9 (cutoff). Put a piece of stock in the chuck. Turned to stoch to 3/4" diameter. Set Part X diameter and Z position.

Loaded the file, pressed cycle start, installed tool #2, Acorn faced the end of the stock and turned the diameters for the Pawn (all went well), Acorn asked for tool #9, went to install it and found the insert had fallen out (couldn't find it, no spares).

Cancelled the job, edited the file to use tool #7 (also a cutoff slightly wider end). Saved the file, reloaded the file, restarted it back with tool #2. Acorn retrace the original cuts, asked for tool #7, tool #7 started to cut in the right place and then seemed to move in -Z direction about 1/4" before stalling the spindle and mangling the tool holder. Pictures and report attached.

1. Plan on re-checking the tool offsets
2. Need to make sure that I am setting the part information correctly, i.e. Z position and x diameter.
3. Found difference in stock size between Pawn in the encoder directory and the NCFile directory (one say to use 3/4" stock the other says 1" stock).
4. Always check that each tool has a good insert before running the program.
5. Get a tool tester to set my tool offset automatically (one on order).
6. Learn how to start at a block in the program and step line by line.
7. Mount my GoPro so I am not trying to hold my phone while running the program.
8. Buy a replacement cutoff tool hold with spare inserts.
9. Find my bottle of Crown Royal and chill out some.

Things that went right: 3/4 of a Pawn, CSS, most of the tool offsets and didn't hurt anything much.

Chuck

[cnckeith]

and you can add to the list...
First...
- dry run any new part program (that you haven't already run a hundred times)
- dry run any new tool or resetting tool offsets
- dry run after setting/resetting any new Z 0 or X 0 position
- dry run after re-homing the machine

[cnckeith]

is the X turns per inch correct? 10.4148?

[carbuthn]

I did do a dry run before attempting the first run by running the file as an air cut. Next time I will run to thin wall PVC pipe first.

I also compared the tools to each other. I will find the proper G code to move each tool to the same spot on the Pipe.

The X and Y turns are almost the same and were set using a digital indicator. The machine specs should be the same as the Centroid test lathe. I started with the number from the Techno lathe spec which said 2.5mm per revolution of the ball screw. Measuring with a ruler showed almost 10 threads per inch. (10x 2.5mm = 25mm or 0.9842") I set for 10 turns and then used Marty's spreadsheet to get the actual turns to move 1".

One area I didn't find any information on was where to set the Z offset for Diamond tool that moves straight into the work piece, such as a threading tool, also I set the cutoff tools to the right side of the blade, with the right edge even with the end face of the stock.

When I tried to manually cutoff the Pawn, I was getting a lot of chatter on the cutter, I tried changing speed, changing the cutter height and feed rate with lubricant. No luck, ended up using my 13" Cincinnati Hydro-shift Lathe.

A video or checksheet for commissioning a new machine may help, I didn't find one when I searched for one. I will try to keep enough notes to at least make up a checksheet to help out others.

Thanks for all of the help,
Chuck

[carbuthn]

I did find that I set the Radius (should be 0.000) and the Cutoff tool to the wrong Z position (left side of tool against the face of the stock) I had the right side of the tool even with the face of the stock.

As I understand it, the radius should be 0.000, the Tool against the face of the stock, set the Z offset, select incremental readings, put a - 0.125 or the width of the tool.

Chuck

[cncsnw]

Whether you set the Z offset of a cutoff tool on the left side or the right side is a matter of personal preference.

If you set it to the left side of the blade, then your procedures are more consistent, and you know that the tool will not get any closer to the chuck than the Z value you program it to cut at; but when you program a cutoff, it will need to be at Z-[part length + blade width].

If you set it to the right side of the blade, then when you program a cutoff, you can just use Z-[part length].

[cncsnw]

More important than a dry run, in my opinion, is to use the feedrate override and feed hold on the first part you cut.

Every time each tool is moving in from the tool change position towards the part, slow it down with the feedrate override, and when it is less than a half inch away, stop it with Feed Hold. Then look at the Z and X numbers on the DRO, and see whether they agree with the daylight you see between the tool and the stock. If the cutoff blade is 0.25" away from a 0.75" diameter part, then the tool tip is at a diameter of 1.25". If the DRO says X is at 1.75", then you know the tool is going to go too deep, and you can cancel before anything bad happens.

[cnckeith]

absolutely! i call that the "reality check".... feed hold to stop and look at it...ask yourself does the DRO match the tool position in reality? before proceeding.

[carbuthn]

Thanks for the information,
I will add the tips to my list of things to do before running a part.

I am currently trying to write a program with Intercon that will have me load tool #1, to Z =0.0 of a piece of PVC pipe that I have set the part zero for, and to the diameter of the pipe for the X axis.
It will move back to the tool check (or safe position, not sure how to call tool check with intercon yet), have me change tools and move back to the same position that I had for the reference tool. It will cycle tools until it has checked all of the tools.

The tools should come to the same spot as the reference tool on the PVC pipe. At least that is the plan.
Chuck

[carbuthn]

Some more questions:

1. In the first attachment, I was working on an Intercon file to check the nine tools that I currently have in my tool offset library. The question is why does the end X and Z positions on the left side of the screen show the start X and Z positions from the right side of the screen?

2. I wanted to pause the run before the tool change (check tool position maybe M00). How can I make the program pause before going to tool check position? Inside of a Intercon block? I could add it to the CNC file after the post, but I would need to do this after each edit/post.

3. Tool #7 and #8 go to a Z position that has the left side of the cutoff tool even with the face cut (end of the stock) and then move in the minus Z direction the width of the cutoff tool. Tool #9 moves until the right side of the tool is even with the end of the stock (what I wanted it to do, the displays shows an end position of .0001, could not enter 0.0, this is what I had entered in the starting Z position) like the start and finish Z also X are swapped between the two sides of the screen and the cnc file.

Thanks,
Chuck