Tool Change Macro Help

[Measurement10]

I have a Taig CNC Mill running Acorn. It has an ER16 collet so it would follow a "router style" tool change routine from Centroid's recommendation. Due to the fact im using Fusion360 Personal i am only allowed 1 tool per program. My Z Home sets my tool reference point (as enabled).

My current Tool Change routine:
1) Start-up machine, physically insert Tool 1
2) Go to Tool Offset Table, under Tool 1, hit auto measure. I have a fixed location tool setter and homing switches.
3) Set WCS/Part location using prompts, making sure to put Tool 1 into Z Offset Measurement.
4) Load Program 1 (calling for Tool 1). Run, finish.
5) For a tool change: Load Program 2, install Tool 2
6) Go to Tool Offset Table, under Tool 2, hit auto measure.
7) Run Program 2 with Tool 2.
8) Repeat process for additional tool changes.

Im hoping to simplify this procedure to the following:
1) Start up machine, insert Tool 1
2) Set WCS / Part location using Tool 1 and leaving "Tool 0" in the Z offset measurement (since i sometimes forget). I need to be able to initially manually set Z0 this way since im using flood coolant and touch plates are out.
3) Load Program 1 utilizing Tool 1. Run, finish.
4) For a tool change, Load Program 2, install Tool 2
5) Prompt comes up asking "Would you like to 1) Auto Measure tool or 2) Manually Measure tool". Manual measurement is for off-center tools (fly-cutter, etc).
6) Macro auto measures tool or lets me jog tool to Touch Off device.
7) Start program, finish.
8) Prompt repeats when loading additional new Programs.

Im currently going through the macro details in the CNC12 manual but it's a bit complicated for me. Is there anyone that could help with a suitable macro?

[cnckeith]

are you currently using a custom macro? if so, post it here.

along with a fresh report.zip so we can see your cnc control configuration setup.

[cnckeith]

which tool measurement method do you want to use? reference tool? or Z home = Z ref (measure from Z home)?

also if the cad cam system only lets you post a program with one tool you can "join" the programs together like this.
open notepad ++ and create a "master" program for your part.

mastermypartnamehere.cnc

then type out

M6 ; a custom M6 macro that asks you to tell CNC12 what tool is in the spindle and then will touch off of the top of the part or a TT which ever method you want
M98 "name of first program.cnc" ;this program uses tool 1
M6
M98 "name of 2nd program.cnc" ;this program uses tool 2
M6
M98 "name of 3rd program.cnc" ;this program uses tool 3
etc..
etc..


then press F2 Load to load "mastermypartnamehere.cnc" and then all the little programs run as one continuous program you don't have to go and load each one.

this is just one way of doing this.

i do this all the time for various reason like easily being able to skip over a set of operations or easy to change the order of machining as well as joining individual program that have been individually sorted out into one part program.

[Measurement10]

Thanks Keith! I found a plugin called "Post Process All" which does the work for you. Have you tried this? It notes compatibility with Centroid’s posts. Looks intriguing but I might just do it manually for now like you suggested, inserting M98 + M6 between each setup. Here is the link if you're interested, https://github.com/TimPaterson/Fusion360-Batch-Post

My machine report attached.

Since i am using a collet style machine without tool holders (router style tool changes) Z Home = Z Ref.

Should I be using the Fixed Tool Touch Off = Z Ref or keep Z Home = Z Ref? Im not sure of the benefits of either...

I've read the macro programming guide and assembled my own tool change macro... and it works! My intention was to create a prompt that asks me if i want to 0) Keep Z0 as-is 1) Automatic Tool Touch Off or 2) Manual Tool Touch Off (for Fly-cutters, etc). Going to test it some more...

[suntravel]

I would go another way, since I am too lazy to measure each tool change

Use ER16 shrink fit collets, perfect same tool length after a change

https://shop.haimer.com/us/Shrink-Fit-C ... 160.020.05

Uwe

[Measurement10]

How much are those?

[suntravel]

How much are those?

Too expensive for hobby, since you also need a shrinkstation.

But there are cheap DIY ways, like shrinking a ring on the tools, or use an internal stop in the spindle...

Uwe

[Measurement10]

I was looking into this but worried about deflection due to longer stick-out with the end stop, also not sure about vibration issues with 10k rpm.

[Measurement10]

So looks like the macro is working however there is a new problem. After the tool is measured and goes back to the workpiece to start cutting, its at the height of the tool setter (because i set that as new Z0). Problem is its not at the correct height- its cutting in the air.

When i start up the machine I set the part Z0 using the first tool, an end mill in most cases. For the first tool its no problem, i just select 0 (do not change Z0 value when prompted). However for the additional tools its a problem. Incorrect Z height.

How can i program it to keep the original value and subtract or add the offset of the new tool?

[Measurement10]

Ok, i think i got it. I realized that although you set up the part initially and set Z0 using the initial tool, the initial tool still needs to be touched off using the tool setter (unless im wrong about this). I guess it keeps the Z0 and touch off values separate, the initial tool touch off value is still needed for subsequent tool measurement offsets.

From what i've seen in the previous macro's, even though there is a touch plate, the initial tool still needs touching off. From this evidence I wrote into the macro to account for initial and subsequent tool changes. The initial tool can be automatically or manually positioned and touched off and subsequent tools can be automatically or manually touched off. I tested it and it works well. If anyone can think of a way to shorten this macro, perhaps eliminate the need for the initial tool touch off it would be helpful.