Bit setter macro v2.0

Hi Stephane,

To modify where on the machine the router stops you would modify the fifth line in both portions of the macro G53 G0 X780 Y50. Just change the X and Y to wherever suits you this is best done immediately after homing the machine. Move the router to where you like and then use the coordinates the display is showing as the new values on those lines. I put way in the corner just to maximize work area. There’s actually no reason that there couldn’t be a pause added to the middle, change bit and then continue to the corner as well. So many ways to do this it’s all about what works best for you.

Keep in mind depending on your setup the Z values might need some modification as well. Also, this version will want to measure the tool length every time you start a file. There is a different version posted that probes only if you have a tool change but requires that the old tool and the new tool are measured.

This video shows the other macro in action.

Feel free to message me if you have any questions, I’m on the 1F FB group and can be reached via Messenger.

Hope this helps!

3 Likes

Hi Dennis,

I haven’t done any work in Fusion with this machine to this point. I have used it to make some clamps and such in the past.

This macro actually gets put into the controller not the gcode file. Having said that I suppose it could be added to the file itself would just need to be careful about where it was inserted.

So, you should be able to remove the M2 command at the end of the first gcode of file and then add an M6 command and paste in the next gcode, and continue this process with subsequent tool paths. I’ve only ever done single tool work with Fusion but would assume there should be a way to build files with multiple toolpaths instead of having to copy and paste.

If I get some time in the next few days I’ll play around with Fusion and see what works.

Is there a 1F post processor for fusion? If not which one have you been using?

Ho Lee Krap, dude! I do a lot of 2-sided 3D items and this looks like it will solve a lot of difficulties! Mad props!

1 Like

Awesome glad it will help. Just be careful of the Z values if you’re using a spindle or in a different mounting position than the lowest you might need to make some adjustments. If you need any help feel free to reach out!

Cheers

This is great Mike! I am a long time app developer so this is a whole new language for me to learn! I did notice that you are setting the macro to MM is it going to matter if the system settings are in inches and using an inches post processor. Or does the firmware convert everything to MM anyways in the back ground. Thank you in advance for you info.

Hi Scott,

In my experience it doesn’t matter the M70 command is suspending the modal commands. The factory settings are in MM so I didn’t actually give it any thought but haven’t heard of it causing any issues for anyone.

IMO you are better off leaving the machine in metric. Of the 2 machines I’ve owned metric is native. I’ve seen some issues with some software not working properly when saving toolpaths on the FB group and almost always comes back to an metric/imperial issue with the post processor.

Here’s a link to a different thread in here with a bit different version of this with some explanations of what each line is doing.

Hi all,

I have a project that uses 2 bits and I saved the toolpaths to 1 file.

Am I wrong in thinking that when I generated the gcode from VCarve Pro using the Onefinitty PP, there should be some M6 codes in the file for the bit change? If so, I must be doing something wrong because there are none.

Just trying to wrap my head around the whole concept.

Thanks

Surprised there isn’t a tool change prompt however you have no way to zero the bit or raise the router with the normal default setup so it is best to save one file per tool

Yes there should be one M6 per tool change command. But as @Hermsen.BJ pointed out unless you’re going to use the bit setting macro I wrote it can be challenging to make bit changes work with factory M6 command. I’ve been using the macro for a 2 or 3 months now and love it.

I’ve found probing between tools manually can lead to some variation in DOC between tools. The macro is VERY accurate for DOC.

In V-Carve, if you put multiple tool paths into a single file, the M06 is present. It allows you to change tools, put the probe underneath the tool, and it will probe for Z. The “home” position in the material setup will be used to “park” the router for the tool change - so you can raise the Z height there, and have plenty of room to change the tool. The only issue is that you can’t move anything during the tool change - so -0,0 will be used as the spot where the Z probe will happen, unless you put something different there.

Once I figured out how to set the Z height at tool change, this has worked very well for me.

1 Like

Darned idiot I am. :slight_smile:
I was looking for M6 and not M06.
Found the tool change prompt.
Can’t wait to get my machine. It should be here next week some time.

Mike,
I added your G-code and it works, sometimes. Depending on the file I load, I get this error:

Any ideas how I can fix this?

Can you send me a screen shot of the code entered into settings in the controller? Also, which version are you using?

I have not had any errors of this nature. The only thing I’ve found is Z will often say over or under but in now way effects machine running.

Hi Mike,

When the macro prompts for tool changes, is it possible to have the macro tell you the actual tool to use?
At the moment, it simply says “Change Tool”.
In multi tool carves, it would be very convenient to be told which tool to insert in your router :slight_smile:
I use the tool numbers as I have assigned a number to each tool in the database.

Thanks

1 Like

Well, that’s a a yes and no. I modified the PP for Vectric to have it display the next tool number in the first dialogue box. So if you’re using the macro version that measures both tools at tool change it will show the tool number before the first measurement of original tool not when prompted to change tool for the new one. It’s better than nothing I suppose. If you’re using v2.0 that measures only new tool at tool change then it would display tool number at the correct time.

I am pretty sure I am using the V2.0 of the macro.
But I think I am using the default PP from OF for VCarve Pro.
I am using firmware version 1.0.7 that came with my machine.

I will go through the process later today and take notes of the steps I see.

I will get back to you.

2.0 measures the tool before you start the program and then measures the new tool only at tool change in which case, yes the PP can be modified to show new tool number.

I think this would be the relevant section in the PP:

±--------------------------------------------------

  • Commands output at toolchange
    ±--------------------------------------------------

begin TOOLCHANGE

“G0[ZH]”
“G0[XH][YH]”
“M05”
“M06 T[T]” <<== Is this not representing the tool number? [T]

Yes, it’s been a while I’ll check the exact command when I get home and post it. You need to add a M0 message and it will display in the dialogue. I think it’s “M0(Insert Tool [T])”. After the M06 line, I’ll confirm with you later.

@stleroux
Sorry I was off on the line for displaying tool number. Here’s how I have it and it will display tool number in dialogue pop up. Again if you’re using v2.0 it will show up at the right time. If you’re using the original macro that measures both tools at tool change it will show tool number on the first popup, instead of the second one. Not sure why I thought it was M0, sorry.

±--------------------------------------------------

  • Commands output at toolchange
    ±--------------------------------------------------

begin TOOLCHANGE

“G0[ZH]”
“G0[XH][YH]”
“M05”
“T[T] (MSG, Insert Tool [T])”
“M06 T[T]”

Hope this helps!

Cheers,
Mike