Mixing manual and automatic tool changes - In Program

[Bob La Londe]

Is it possible or practical to mix automatic and manual tool changes in program. Do all your automation at the beginning, and then at the end do your short operations when standing over the machine is no big deal. ie: surface, machine, 3D machine, etc, then at the end if you need more than ten tools manually swap tools for drill and tap operations with tools that are not loaded in the tool holder. I know it could be done easily enough by running two separate code files, but the limitations is I could forget to run the second code file seeing my beautifully machined part and take it off the fixture or out of the vise loosing position and then having to waste time relocating it to finish the job.

What happens if you execute a code file that includes tools that are not preloaded in the ATC? (They would be loaded in the tool table.)

I have reviewed a lot of my jobs, and its very rare that a job requires more than ten tools, but it does happen. If I incorporate some of the things I do manually now I'd use up 5 tools just for drills and a tap. My little high speed machines do interpolated spiral milling pretty fast, but it is still faster to just use a drill bit at the correct speed and feed rate. I use interpolated milling to (sometimes) avoid a tool change since the baby Speedmasters are strictly manual tool change and touch off.

Similar Threads:

• Need Help!- Manual Tool change under Mazatrol program
• Need Help!- Automatic tool changer program for a 8 tool turret Diy lathe cnc
• Need Help!- Help with mods to this Automatic Manual Tool Changer
• manual automatic tool change
• Manual Automatic Tool Change

[109jb]

Back when i made a living running VMCs we would have occasions where we used manual and automatic tool changes. With a 30 till carousel it was most often because we had a tool that was physically to long to fit in the carousel. So, i would say if you have a need then go for it. I can't see a reason not to. It was a long time ago, but as i recall, on the Cincinnati VMCs i ranall that was required was calling a tool number larger than the carousel capacity. For example with a 30 tool changer calling tool number 31 would cause the machine to executea manual tool change.

Sent from my RS988 using Tapatalk

[Bob La Londe]

Back when i made a living running VMCs we would have occasions where we used manual and automatic tool changes. With a 30 till carousel it was most often because we had a tool that was physically to long to fit in the carousel. So, i would say if you have a need then go for it. I can't see a reason not to. It was a long time ago, but as i recall, on the Cincinnati VMCs i ranall that was required was calling a tool number larger than the carousel capacity. For example with a 30 tool changer calling tool number 31 would cause the machine to executea manual tool change.

Sent from my RS988 using Tapatalk

Not sure it will work that way with PathPilot. According to their video on loading the tool changer you can have any tool number from the tool table in any slot on the tool changer, and PathPilot will manage it.

[109jb]

According to the Tormach manual,

If your program requires 11 or more tools, the ATC will change tools automatically
for all tools in its tray, and pause for a manual change for tools that are not assigned to the tray.

So, the way I read that is if you don't associate a tool number with a tool tray position it should prompt for a manual tool change

[CadRhino]

Yes, the machine will wait for you to manually load the tool.




QUOTE=Bob La Londe;2159496]Is it possible or practical to mix automatic and manual tool changes in program. Do all your automation at the beginning, and then at the end do your short operations when standing over the machine is no big deal. ie: surface, machine, 3D machine, etc, then at the end if you need more than ten tools manually swap tools for drill and tap operations with tools that are not loaded in the tool holder. I know it could be done easily enough by running two separate code files, but the limitations is I could forget to run the second code file seeing my beautifully machined part and take it off the fixture or out of the vise loosing position and then having to waste time relocating it to finish the job.

What happens if you execute a code file that includes tools that are not preloaded in the ATC? (They would be loaded in the tool table.)

I have reviewed a lot of my jobs, and its very rare that a job requires more than ten tools, but it does happen. If I incorporate some of the things I do manually now I'd use up 5 tools just for drills and a tap. My little high speed machines do interpolated spiral milling pretty fast, but it is still faster to just use a drill bit at the correct speed and feed rate. I use interpolated milling to (sometimes) avoid a tool change since the baby Speedmasters are strictly manual tool change and touch off.[/QUOTE]

[shred]

The ATC pauses with "Put tool #17 in spindle and press cycle Start" message and then "Remove tool #17 and press cycle start" when its time for the next one. The only tricky thing is if you're trying to re-use toolholders or a drill chuck or something like that since you don't get a chance to mess with the offsets when that's going on.

[74BurkeMVN]

I do this a lot, most times if I don't want to unload tools already in the tray.
If the tool is not in the ATC, PathPilot will stop after automatically unloading the spindle and prompt you to load whatever tool number you have assigned that is not in the tray. If nothing was in the tray it would prompt for every tool in the program.
One thing to note, when the "hand changed" tool is finished and it's time to manually or automatically change for another tool, you will not have sufficient Z clearance to remove the hand loaded tool unless you have thought ahead in CAM to program enough "clearance height" or manually edit-in a G30 (which is what I do). It would be nice if PathPilot recognized this situation and at least automatically went to the programmed Z height of the ATC.
If you forget to program in clearance, you can always stop the program (escape key) and then manually jog to remove, then right click on the tool/operation line of code you want to pick back up on and choose to set that as the start position.

[Bob La Londe]

I guess I could modify my CAM post to insert a G30 before every tool change. Its not going to hurt anything.

P.S. What's the difference between G28 and G30. I use G28 for the tool change location in my tool change macros in Mach 3. Goes to the location set in configuration. The definitions I see seems to indicate they are the same.

~~~ Be right back ~~~

Ah, in Mach G28 goes to a set homing location and G30 goes to absolute home. G28 also uses safe z moves if safe z is turned on. G30 does not.

So can you set a G28 location in PathPilot?

Does it implement a G30 as a linear move or can it be set as a safe move like G28 with Safe Z moves turned in does in Mach? If it performs a linear move you could have circumstances where it crashes. They would be very rare, but its possible. You would have to set your clearance height to clear all possible obstacles. Might make for some awfully inefficient code in some cases.

My machine doesn't get here until late next week and I figure it will take me a while to get it going, but I want to have an idea what I am getting into before I run my first code.

[74BurkeMVN]

If you use Fusion360, the Tormach post has a configurable option to insert a g30 between tools automatically.
Not sure about the g28...

[soymilk]

G30 is 2nd reference point.
G28 is z home position

G28 will take the mill all the way to the top. I could be wrong but I believe the g28 position is based off the limit switches.

G30 is generally where the tool changer will go to change tools and still have z travel for the tool changer to work

All extensive purposes you should probably change your post to G30. But you can still use g28. All it will do is move back down for tool changes.

[Bob La Londe]

G30 is 2nd reference point.
G28 is z home position

G28 will take the mill all the way to the top. I could be wrong but I believe the g28 position is based off the limit switches.

G30 is generally where the tool changer will go to change tools and still have z travel for the tool changer to work

All extensive purposes you should probably change your post to G30. But you can still use g28. All it will do is move back down for tool changes.

I guess I'll have to experiment with PathPilot to know for sure. That is reversed from Mach based on the experiment I did yesterday. I walked out to the shop in the middle of my last post and tested it on a machine. G30 went to 0,0,0 absolute (machine coordinates) in a direct line from where ever it was in actual testing and I know for a fact G28 (in Mach) goes to the programmed or set homing location set in homing and limits using a safe Z move if you have Safe Z moves turned on because I use it every day. I also recall in a Tormach video many years ago when they still used Mach that they used G28 inserted into the code. I always thought that was silly because you had to modify your post processor to do that. If it was in the tool change macro which is how I do it then the default post processor worked fine for most Fanuc compatible CAM packages or those with a Mach specific post. I noticed when I started using Fusion360 they inserted a G28 in the Mach post processor as well as an optional stop M code. I had to remove those as it was annoying to have two stops in my program. One inserted and one in my macro. What was really annoying was when my copy of Fusion updated they put those back in. I thought there was something wrong with my machines until I fixed it again.

Actually, I have modified a couple of my tool change macros to use G53 moves instead of G28 for machine specific reasons. I also store the current offset location before the move, and return to it after the tool change so that in those rare instances when CAM doesn't put out all coordinates because one or more of them is the same as the end of the last command it doesn't result in a crash.

Ie:

G01 X5y5 F20
G00 Z.05
T6 M6
G01 X5Y7 (may only put out (G01 Y7)

[soymilk]

Its not quite opposite as you describe for G30. G30 is just a user defined reference point. On your mach 3 machine, it went back to 0,0,0 because thats probably whats defined in the system parameters. It works the same way in mach 3 or pathpilot. Keep in mind on pathpilot, when you use G30, it only moves in the Z axis.



you sure like going off on tangents there haha . In the past I've had rare issues like what you described with cam systems not reinstating positions because it thinks its already there. I fix that in the post so it always outputs the X and Y location at the top of each new tool block. It was a problem with text based cam systems like compact II.

[Bob La Londe]

Its not quite opposite as you describe for G30. G30 is just a user defined reference point. On your mach 3 machine, it went back to 0,0,0 because thats probably whats defined in the system parameters. It works the same way in mach 3 or pathpilot. Keep in mind on pathpilot, when you use G30, it only moves in the Z axis.

you sure like going off on tangents there haha

. In the past I've had rare issues like what you described with cam systems not reinstating positions because it thinks its already there. I fix that in the post so it always outputs the X and Y location at the top of each new tool block. It was a problem with text based cam systems like compact II.

Not really. Its all related to tool changes and how they perform. One reason I was asking was because another user (using PathPilot for a non-Tormach) mentioned to me that he has to STOP code execution in order to jog his machine for a manual tool change. Its all related. Too be fair I am prone to tangents, but not really in this thread.

I'll have to look then about the G30 because G28 is definitely a user defined point in Mach. Like I said I use it every day in my M6 macros even if its transparent to my code. I wouldn't mind a simple Z retract for a manual tool change though. Its very rare I would be using a tool so long or a part so tall I couldn't change it.

I resist changing CAM posts if I can help it so I don't have to remember all the changes when the software updates. Sadly, sometimes there is no choice.

[Bob La Londe]

I just got called by the trucking company before lunch. The mill and stand should arrive tomorrow.

No word on the rest of the order.

A second order of accessories will get here on Monday.

[soymilk]

#5284-#5303 should control G30 for Mach3


Working with mastercam and Nx, I try to hold off updates if I can. I will post a sample file with the software before post and post a sample file with the new update. Then I run it through a program (notepad++) to compare the two programs. 99.99% of the time it doesn't affect the program. Usually patches fix functionality within the cam system itself. I can't say the same for fusion360 as I don't work with it much. General practice is to change the cam and not the subprograms in the machine. But that's in a large manufacturing setting. Your machines your rules. Whatever floats your boat.


Have fun putting it together. I had a blast putting mines together. I wished I had taken things a little bit slower. Thinking about it now, I wished I did something to help prevent shavings from going under the machine between the machine and the stand.

[Bob La Londe]

Oh, I get that's the norm for some reason, but think of this., Tool changes are a machine specific operation. They are only done that way on that machine. Sure you could have more of that one machine, but if you do a lot of custom work like I do its more likely to have different machines that do different things well because its cheaper than one machine that does everything, and those "not everything" machines can be powered in a small shop and perform multiple jobs at the same time. At the moment I have 5 CNC machines that run. (one I am working on, but..). Three of them are functionally very similar, but the other two are quite different. It just doesn't make sense to have different post processors for each machine just to manage a very machine specific task.

I realize some machine operators and programmers may not see it that way, because for many they do not have the ability to modify the machine. They have to live with whatever the machine builder decided was "good enough." They only have that level of control over their CAM program. Even many Tormach users since many early machines were sold with a locked down version of Mach. I don't know yet how locked down Path Pilot is. I didn't come from a background of dialed in, pre-setup, and locked down machines.

I started with pieces of a Taig CNC system in multiple boxes with a POS Xylotek knockoff controller and had to learn to tweak modify and adjust every thing to make a few parts. I used that thing to make tens of thousands of dollars worth of parts eventually, and some day I'll put it on a stand in my office. If I didn't learn to make the machine work I wouldn't be here. Its just a machine. It will bend to my will. To give you an idea how different mindsets can be in machining there are guys who will say to never ever modify a vise no matter what. Sure use soft jaws if you must, but never touch the vise under penalty of forever being labeled a pariah and never being considered a "real" machinist. I have purchased vises with the specific intent to throw them on the big mill and cut them before they ever see a part. If I hadn't I would not have been able to quickly and easily make use of the full working envelope of my little high speed machines. A bigger vise wouldn't work. It wouldn't fit in the factory cabinet and use the full working envelope, and if it did it would hit the column.

So no I do not think a machine specific operation should be managed by software twice removed from the machine. I think the machine should be setup to manage its own machine specific operation so it doesn't crash or create a totally avoidable condition where it has to be stopped in order to continue working. All my CAM software does now is say change the tool. The machine changes the tool or accommodates changing the tool, and it makes sure it doesn't screw up the job because it remembers where it was before the tool change and it goes back there (with z offset changed appropriately). I started out with a machine that HAD TO BE changed and setups changed in order to work at all. By making the machine able to manage the same set of commands I can generate more standardized code and make fewer mistakes. In addition the code is smaller and it takes a larger job before it starts to overload the control computer. If your average job takes 20 minutes its no big deal. My average job takes hours, and right now I am still working on a custom job that has taken weeks of machine time and months overall.

An example: (There are many in the real world) If you are a motorcyclist you will know that on modern motorcycles they all have a foot shifter on the right hand side. It was not always that way. It didn't matter if an operator only had one motorcycle in their entire life, but most motorcyclists have many different bikes over their lifetime. The controls were standardized and the result was fewer operator generated crashes.

I realize LinuxCNC is different from Mach. This machine may be "to" different, but I'll find out. By knowing ahead of time what it does and doesn't do I'll hopefully avoid some of those operator generated crashes.

Wish me luck. I'm gonna need it. LOL.