Proper method to specify tool offsets so that PP will call tools as "T0202"?

[EDMTMC]

(I am new to all of this, so please bear with me as I learn. I'm using F360 and Mach3 and a Sherline Lathe.)

As I understand it, Mach3 Turn expects tool changes to be in format T0202 where the offset # matches the tool #. (I think I understand that for Mill, the offset could change but for lathe it';s set to match tool, correct?)

Fusion 360 does not have a default offset in the tool definition. As a result, unless you specify an offset, the F360 Post Processor will post "T02" to gcode, which Mach3 Turn doesn't like (as far as I understand).

I have been able to solve this in Fusion 360 on the Tool Setup Post Processor tab by manually choosing a "Compensation Offset" to match the tool # when the tool is defined.,

If I choose a compensation offset that matches the tool #, then the Fusion 360 CAM Post Processor will generate tool change code in the format "T0202" which is what Mach3 Turn is expecting.

That worked for me. But, I could see plenty of opportunity to mess up -- especially if tools get renumbered!

Is that just the way it's done? Or, should the Mach3 Turn PP be changed to use the tool # as the comp offset unless one is present in the F360 tool definition so that "T02" becomes "T0202"?

I'm thinking that there must be a better way to do this.

I hope someone with far more expertise than I have can can help and I can learn.

[HughesTooling]

---

@EDMTMC wrote:

I have been able to solve this in Fusion 360 on the Tool Setup Post Processor tab by manually choosing a "Compensation Offset" to match the tool # when the tool is defined.,

If I choose a compensation offset that matches the tool #, then the Fusion 360 CAM Post Processor will generate tool change code in the format "T0202" which is what Mach3 Turn is expecting.

That worked for me. But, I could see plenty of opportunity to mess up -- especially if tools get renumbered!

How are you ending up with different number for the tool and offset? I've just tried making a few new tools and the tool and offset stay the same even after a renumber. I haven't experimented with this much because I've setup libraries for my lathes and don't need to change to tool numbers.

Mark

[Anonymous]

---

@EDMTMC wrote:

If I choose a compensation offset that matches the tool #, then the Fusion 360 CAM Post Processor will generate tool change code in the format "T0202" which is what Mach3 Turn is expecting.

But that's what T0202 means for lathe tool changes: select Tool #2, and use Offset #2.  You could have T0203 if you want to use Tool #2 with offset #3.

Imagine perhaps a tool turret with tool holders that can hold 2 drills side by side.  It's still tool #2 on the turret, but each drill would have a different X offset.

Or if you have one of those combination cutoff / bar puller tools.  Or maybe one of those insert drills that you can also bore with.  Guess it really depends on the machine if you'd ever need to use this though.  Just set it up as different tools on a gang tool lathe I suppose?

I'm still working on the retrofit of my little lathe to Mach3, so I haven't tried this under Mach yet.  Works this way with my AhHa controlled lathe though.

If there's never a chance of you needing a different offset though it's a fairly simple modification to make the post use the tool number twice.

Dave

[EDMTMC]

Interesting. Thank you for including the video. I watched it a few times and was able to reproduce your experience.

So, here's what I have learned:

IF you are creating a new lathe tool (and have not touched the compensation offset field) THEN the compensation offset # will track your tool #.

HOWEVER, once you touch the compensation offset field, thereafter it will no longer track the tool #. So, you will have to maintain it manually from then on.

If you renumber your tools this could be a problem, but I guess that is something to remember.

For me, since I do not run lathe that has a tool changer with multiple tool positions where the offset would be used, I think I'd like the peace of mind of knowing that the post processor will always force the compensation offset # to match the tool #. (I am new at this, so if what I am asking is unwise, I welcome feedback).

I have attached my Mach3 Lathe Post which I got from the Fusion360 web site. It's for Artsoft Mach3 Generic Turning and dated 8/22/2016. It works.

Do you (or another reader) know how to modify this post to force the tool offset # to always match the tool # so that T01 becomes T0101?  (Regardless of what may be programmed into the F360 Tool library)

[EDMTMC]

Dave, thank you for your thoughtful response. It not only answers my question but deepened my understanding as to what value compensation offsets have on a lathe. So, as a beginner. thank you for taking the time to share.

I also started with an AhHa controll for my Sherline, build by Bill Griffin 16 years ago. It worked, however, I could not wrap my head around the tool chain to go from concept to CNC. Since then, we have forums, youtube and many excellent products to help (like Fusion 360) so I dusted off my Sherline and replaced the AhHa control with Mach3 and PMDX, ESS, and G540. They work great.

Now I am teaching myself the tool chain with Fusion 360 to go from CAD to CAM to CNC to Part.  I actually have it working!

Dave, you wrote: "If there's never a chance of you needing a different offset though it's a fairly simple modification to make the post use the tool number twice."

I would like to do that. if you will scroll to see my response to Mark in this thread, I have shared the Mach3 PP I am using.

Thanks again Dave and Mark,

Eric Mack

[Anonymous]

Eric,

I definitely recognize the name Bill Griffin (probably from the AhHa Yahoo forum) though I've never had any interaction with him.  I've got a Dyna Mechtronics DM3000H (the bigger floor standing model) that came to me with a mostly functional AhHa control.  This control certainly has it's share of idiosyncrasies, but at least it takes some flavor of gcode not like the original Dyna SKIP control that I'm lucky to never have had to use.  I would love to move to either Mach3 or LinuxCNC on this machine, but it has quite a bit of extra I/O for the pneumatic collet closer and tool changer so I'm going to be happy with it for now. 🙂

I would suggest you edit the post processor yourself if you're up for it.  Once you get a look at the code you'll find that most of it is pretty straight forward.

If you don't know, hitting the "Open config" button on the Post Process window will open your post in Brackets.

You're looking for this (should be line 484) line:

    writeBlock("T" + toolFormat.format(tool.number * 100 + compensationOffset));

This is the line that puts the "Txxxx" command in the gcode.  It writes the letter 'T' and then toolFormat.format tells it to use the defined (on line 68) format for the number inside the parenthesis.  The format is defined as no decimal places, and padded out to four digits with zeros.

That number is just the tool number * 100 (to bump it to the left 2 places) plus the compensationOffset.  So for tool #2 with the compensation also set to 2 it's 200 + 2.

You want to guarantee that it's always tool number * 100 + tool number. So just change the line to:

    writeBlock("T" + toolFormat.format(tool.number * 100 + tool.number));

Note: if you look around the post a bit more you'll see that the "T" + toolFormat.format is actually used in two more places.  However, those are only used if the properties.preloadTool is set to true.  I'm pretty sure that Mach3 doesn't support preloading tools, and even if it does it means nothing without a tool changer.  But if you ever accidentally set that property to true now you' can see what will happen.

Note #2, I haven't tested this change so there's a very small possibility that it won't work.  But not really with this simple of a change.

Please let me know if this doesn't work though.

Dave

[daniel_lyall]

If you use notepad++ to edit posts it makes life a lot easier as you have a menu to the sections in the post and everything is colour coded and get NC Corrector it's a free backplotter.

[HughesTooling]

One more piece of advice. 

Do not put custom posts in the generic posts folder. Use the personal folder. or another location.

Fusion 360 CAM Personal Posts Folder Locations

_______________________________________________________________________________

Microsoft Windows:
%appdata%\Autodesk\Fusion 360 CAM\Posts

Mac / Apple / OSX:
/Users/<user id>/Autodesk/Fusion 360 CAM/Posts

Mark