[LeeWay]

Okay guys.
I never really homed my machines before. At least not my mills.
Always do my plasma and router and set my homes to sync coordinate systems in the lathe.

Problem 1. I am learning to use Fusion 360. I really like it so far. Not to difficult to pick up. I am further along in it than in SW and HSMXpress, but I think both are similar enough that I will be able to equal the knowledge out at some point. Both have features that I like.
When I home the machine, it goes to the top of Z first. I take it that this is normal. My problem is then that this becomes the normal tool change position as well. Then when I have a tool that is long, it cannot go up high enough to implement that tool and the stepper stalls. Since 360 does not have a place to input the actual TCP, I guess it defaults to home.
My longest tool is nearly 3.5" taller than my shortest tool. Is there a way to offset my Z Home position?
Well all three axes for that matter.

Also there are definitely some parameters that need changing in the Standard Mach 3 Post processor in Fusion 360.
I will work with them on getting that done.

It outputs all the tools needed for that job to start with. I know what tools I have available and program everything according to that tool table.
I don't need that stuff in there except when it's calling a tool.

It also outputs the tool # and it's offset on different lines. Mach 3 doesn't like that either.
It also creeps at like 6 IPM to home and to tool change as well as when applying the tool offset. That's Granny slow.

And at tool change, you have to hit cycle start twice. The first time does nothing really that I could tell.


Anyway I will have to get used to homing this machine at start up to get prepared for bigger and better things. (Ray, you listening)

I'll look for the offset thing from Home and post a follow up.
Just thought you guys might like to know about this stuff.

[LeeWay]

Okay.
I think I solved the offset issue. It is the G54 offsets in the offsets page, correct? I had them set to zero, so I assume that meant home. If I have an offset in there like Z -4.00, will it go to zero at the top first and then back down?
Guess I will find out. No nice tools in the spindle for this one. Just an FYI for guys with the Pulsar,don't start the spindle without a tool in the collet unless you like seeing R-8 Collets dancing around inside your enclosure.

[ger21]

G54 is the default coordinate system in Mach3.
When you zero an axis, you're actually setting a G54 offset, which is relative to the machine coordinates. Machine coordinates can only be zeroed by homing the machine.
If you have no home switches, when you home the machine, it will set machine coordinates to zero at the current tool position.
Then when you zero your axis, it will set G54 offsets relative to the machine coordinates.

I had them set to zero, so I assume that meant home.

It's 0,0,0 in machine coordinates. That's typically called home.

If I have an offset in there like Z -4.00, will it go to zero at the top first and then back down?

No, it just makes Z zero in the current coordinate system -4 from Z zero in machine coordinates.

I suggest you watch the home, limits and offsets video at machsupport.com, where Art explains all this stuff.

I ordered all the components for a new PC today, and hope to be able to start playing with Fusion 360 in two weeks or so. I should be able to help with the post then. Right now, I'm using a PC with XP, and can't run it.

[amish_rabbi]

any chance you could just modify the post to tell it to just do a Z move when you call a tool change?

a "wrong" way to do it that I can think of takes advantage of the fact that if you don't home your machine when you turn it on your machine co-ordinates set 0,0,0 to wherever your spindle is on start up (at least it did for me, I found this out by accident, happily nothing broke). so jog to wherever you want to do all your tool changes, then restart the machine/mach3 and hey new home position for your tool change

[LeeWay]

That is what happened today when I cranked it up first. It was set to zero on the last job.
I raised it up to air cut, then zeroed like normal. The difference was I ran the first code produced by 360 and it called the G54, so back down to start up position. Scared me kinda. It stopped correctly though. Then homed it.
I am still working that part out, but will post back my findings. Thanks, Guys.

Gerry, 360 still has a few issues of course, but they have teams of guys implementing new stuff and ideas and features as well as actively correcting bugs. Like Les with SheetCam and Art with Mach 3 before he semi retired, they are listening to the users and taking care of what needs doing. That is priceless. I would suggest going through some of the videos on Youtube. They are pretty good. That will get you drooling over it.

[LeeWay]

I guess I'll have to give that video a look.

A few issues. My X axis doesn't home. It says the home switch is engaged when it isn't. I do not remember disabling that switch, but it was. It would home Y and Z. I'll have to get that fixed. John is supposed to be sending me a new BOB. The Arduino type at some point. I did replace the switch with a brand new one and that didn't solve the issue.

It may be in the BOB itself. I had trouble with the X switch in the Torus too.

The machine stopping at nothing that I mentioned before was for an M1 call in the Gcode.
I haven't seen that before and didn't realize I had it set to on in the General Config by default.

Changed that and now it acts as it should at tool change. Not where I want it though.

The G54 offset does me no good actually. It still homes at the top of Z and still stalls on tool changes with long offsets because it keeps trying to go up.
I think I would have to physically move that switch down. Not sure at this point. Definitely have some issues to work through.

[SCzEngrgGroup]

Okay guys.
I never really homed my machines before. At least not my mills.
Always do my plasma and router and set my homes to sync coordinate systems in the lathe.

Problem 1. I am learning to use Fusion 360. I really like it so far. Not to difficult to pick up. I am further along in it than in SW and HSMXpress, but I think both are similar enough that I will be able to equal the knowledge out at some point. Both have features that I like.
When I home the machine, it goes to the top of Z first. I take it that this is normal. My problem is then that this becomes the normal tool change position as well. Then when I have a tool that is long, it cannot go up high enough to implement that tool and the stepper stalls. Since 360 does not have a place to input the actual TCP, I guess it defaults to home.
My longest tool is nearly 3.5" taller than my shortest tool. Is there a way to offset my Z Home position?
Well all three axes for that matter.

You should always home the machine on power-up, so IT knows where it is. The Z home position should be 0.0 in Machine Coordinates, and should be at the very top of Z axis travel. You then set the G54-G59.nnn fixture zero(s) to define where work coordinate zero(s) are.

I would expect any decent POST to move do G53 G0 Z0 in preparation for a toolchange, and I'd bet that is what the POST you're using does. Doing an absolute move in work coordinates is asking for trouble.

I have tools that are as much as 6-7" longer than others, and have no problems.

Also there are definitely some parameters that need changing in the Standard Mach 3 Post processor in Fusion 360.
I will work with them on getting that done.

It outputs all the tools needed for that job to start with. I know what tools I have available and program everything according to that tool table.
I don't need that stuff in there except when it's calling a tool.

I assume you're referring to the tool information output in the comments at the top of the program? Why would you want to remove that? It's perfectly harmless, and helps document the program.

It also outputs the tool # and it's offset on different lines. Mach 3 doesn't like that either.
It also creeps at like 6 IPM to home and to tool change as well as when applying the tool offset. That's Granny slow.

The G43 Hn does NOT need to be on the same line as the M6 Tn. Mach3 should not care. It also does not matter what order they appear in.

And at tool change, you have to hit cycle start twice. The first time does nothing really that I could tell.

The POST is probably outputting an M0 for the manual toolchange, and you probably also have Mach3 configured to pause on toolchange. Change one or the other.

Anyway I will have to get used to homing this machine at start up to get prepared for bigger and better things. (Ray, you listening)

I'll look for the offset thing from Home and post a follow up.
Just thought you guys might like to know about this stuff.

[SCzEngrgGroup]

Lee,

You might want to try the below POST as well. It's a simplified version of my custom POST. Re-name it from .txt to .cps.

Regards,
Ray L.

[LeeWay]

Thanks, Ray.
The M1 is what made me think the Tool number and offset needed to be on the same line. Dolphin Turn and Sheetcam do it that way, so I had just not seen it separated before. Once I fixed the M1 thing, tool changes worked normally.

Here is a snippet of code

(DELTA BRACKET FACE FIRST OP)
(6061 ALUMINUM)
(T8 D=0.25 CR=0. TAPER=45DEG - ZMIN=-0.002 - CHAMFER MILL)
(T11 D=0.167 CR=0. - ZMIN=-0.6 - RIGHT HAND TAP)
(T14 D=0.3125 CR=0. - ZMIN=-1.2 - RIGHT HAND TAP)
(T16 D=0.142 CR=0. TAPER=135DEG - ZMIN=-0.8294 - DRILL)
(T18 D=0.279 CR=0. TAPER=135DEG - ZMIN=-1.3078 - DRILL)
G90 G94 G91.1 G40 G49 G17
G20
G28 G91 Z0.
G90

(TRACE1)
M5
M9
T8 M6
S4500 M3
G54
M8
G0 X1.3568 Y0.405
G43 Z0.4 H8
Z0.01
G1 Z-0.002 F50.
X1.4803 Y0.2932
Z0.01


What I don't need is in red. It is unimportant really, but would clean up the code. I have no need for it to be there.
Where is needs to be if anywhere is dispersed in the Gcode when it is calling for a tool change.

This is how Dolphin and Sheetcam does it. It's what I am used to and that not being there may make a difference. Maybe not.
I always looked at the Gcode on the screen to get the tool number, but it pops up in the Tool Screen on Mach as well.
I suppose I could get used to that there instead.



I agree with how you Z axis homing works. Mach should theoretically work that way too. It doesn't though.
At tool change, it gives you the tool number coming next, however it is still on the previous tools offset. When you get the tool changed, it immediately proceeds to physically move to that tools offset before machining happens again. It won't just do the math and set it in the DRO only. Sooo, it tries to go up from the Home position in Z. It can't do it when home is at the top.

Perhaps it is some settings that I am overlooking or something. Also it moves incredibly slow during a tool change. 6 IPM. Probably a good thing since it's fixin to screw up anyway.

[SCzEngrgGroup]

Lee,

All the stuff in parens is comments, and has ZERO effect on how the program runs. It is put there so when you're setting up the job you can easily see which tools are needed to run the job. To remove them, you'll have to edit the POST. But if you don't like that, you'll HATE what my POST outputs....

Mach homing DOES work like I described, IF Mach3 is configured correctly. Sounds like yours is not.

Turning tool length comp on and off (G43/G49), by itself, does NOT move the head, it only shifts the value displayed in the DRO. The G43 line in your G-code DOES do a move to Z0.4 when it turns comp on.

Again, if you want comp turned on BEFORE you load the next tool, you need to modify the POST. My POST does do this the way you want.

Regards,
Ray L.

[LeeWay]

Thanks, Ray. I downloaded Notepad ++ the other day and it has settings to change the PP's. That info is on the 360 forums.

Your post is totally different.

You apparently have your tool library hard coded. My first tool, which should be #8 and a 45 degree chamfer mill for engraving calls up tool # 2. That is a long drill bit in my library.
Thats as far as I got with it in simulation.

One thing I did notice though is that if I turn off the Z switch as well, then it doesn't move but marks it as homed. That is the work around I am going to have to use until I can get the machine sorted out and dig into why it acts like it does during a tool change.
I gotta say that the Torus did it the same way and my little mill does as well.

[LeeWay]

Okay, turning it off still doesn't work right. Still too fiddly.
I don't recall how hard it is to set the switch lower. If it is like X and Y, then I should be able to slip the slide up or down the bar and lock it where I want. At least a temporary fix.


Man! All I wanted to do was try out some adaptive clearing strategies. Sooo close.

[LeeWay]

Okay.
This is totally off topic. In post #9 above, what color are the two Right Hand Tap comments on your screen?

I highlighted that whole comment section and changed the color to red, but those two lines are showing blue for me in Chrome. Again, unimportant, but it's been that kind of week.

[SCzEngrgGroup]

You apparently have your tool library hard coded.

No, all my tools come out of my HSMXpress tool library, as they should....

Regards,
Ray L.

[SCzEngrgGroup]

Okay.
This is totally off topic. In post #9 above, what color are the two Right Hand Tap comments on your screen?

I highlighted that whole comment section and changed the color to red, but those two lines are showing blue for me in Chrome. Again, unimportant, but it's been that kind of week.

First one is BLUE second one is RED.

Regards,
Ray L.

[SCzEngrgGroup]

Okay, turning it off still doesn't work right. Still too fiddly.
I don't recall how hard it is to set the switch lower. If it is like X and Y, then I should be able to slip the slide up or down the bar and lock it where I want. At least a temporary fix.


Man! All I wanted to do was try out some adaptive clearing strategies. Sooo close.

Lee,

You really should take the time to undertstand how all this is meant to work, and MAKE it work that way. Sounds to me like you've got some pretty fundamental things setup incorrectly, which are likely to cause you endless grief unless you fix them right. Homing is very fundamental, and important, and it's not hard to get it working correctly. If the bar doesn't let you get the switch up high enough, then remove the bar, drill two new holes, and re-mount it where it belongs. It'll take less time to fix it once right, and never have to touch it again, than to work around it now, and then have to come back and re-do it later. And the POST should work fine just as it is.

I set my Z home position to about 1/4" from the physical end of travel.

Regards,
Ray L.

[mmoe]

Okay.
This is totally off topic. In post #9 above, what color are the two Right Hand Tap comments on your screen?

I highlighted that whole comment section and changed the color to red, but those two lines are showing blue for me in Chrome. Again, unimportant, but it's been that kind of week.

I think your topic has been pretty well answered. G53 G0 Z0 at the beginning and end of your program, and you can also add a second line to park the head in a specific place relative to the machining envelope (G53 Xx Yy).

The words "Right Hand Tap" are blue, but I assume that's probably because it's a link to something for sale like other blue text that randomly appears.

BTW, some more off topic, the adaptive toolpaths in Fusion 360 are pretty easy to setup and use, and seem to work very well in general. I get a few odd selections inside the solids I've tested (no idea why as there is no cavity in the solid), so be sure to consider having boundaries ready to go as well if you are working from 3d geometry. I'm finding I have to use boundaries quite a lot more in Fusion 360 than I normally do in Bobcad 3 Axis Mill Pro and the 2d strategies are surprisingly difficult to use directly off the solids if they aren't simple IMHO (the 3d strategies seem to behave as expected much more regularly), but the links between passes in the adaptive clearing and scallop (3d) strategies are really well done and probably one of the best things about the system that no-one will likely really notice. I thought HSM Works was also a Module Works based system, but it's not behaving that way so I now wonder about that assumption. I've complained a lot about the way that Bobcad/Module Works links between passes in the equivalent to "Scallop" (Equidistant Offset in Bobcad), and I swear that Fusion 360 produces exactly what I've suggested needs to happen. On the other hand, I seemed to be the only one who had problems with it, so maybe it's just me. I get way too many dwells that produce perceptible marks when machining in 3d with Equidistant Offset (Scallop equiv.) and I think the linking in Fusion 360 will reduce them pretty significantly, perhaps a 25-50% improvement in surface deviations at those turns. Fusion 360 still a pretty green system and feels like it needs to mature (I manage to get a lot of errors out of it), and it's a ways out from replacing everything I need to do, but it is pretty impressive for sure and about the same level of value at the sale price as Bobcad. I'll be subscribing just to lock the price in with the idea that it may get much better very quickly. I'm not sure I'd say it's worth the $1200/yr they want regularly, but it's definitely worth every penny of $300/yr.

Does it strike anyone else as strange that you can't open anything or save anything in Fusion 360 native format (which would include CAM data) locally? I have some concerns about that given I occasionally work on jobs that come complete with NDAs, and I really don't want to put that data anywhere I can't control. I like the cloud idea for sharing when you want to, and I have no issue with cloud based licensing, but have I missed something or is the only way to interface with your files to store them on their server? That's a pretty huge fail on an otherwise excellent new product. It should be the user's choice whether or not they have to use the cloud for data storage (and you would think better for Autocad if you don't want or need to use their server space).

[mmoe]

No, all my tools come out of my HSMXpress tool library, as they should....

Regards,
Ray L.

I get the same out of Fusion 360. It automatically generates the tool list as comments, and those comments are dependent on the specific program requirements. If you set them up as a specific tool number in Fusion 360, it will show up that way in the comments, so it's entirely custom to each users tool crib.

[ger21]

They are both red here.

I think your topic has been pretty well answered. G53 G0 Z0 at the beginning and end of your program

Make sure you home the Z before you do this, though.

[SCzEngrgGroup]

Lee,

The funky color-coding is likely due to the annoying "Skimlinks" feature of the site, that seems to turn random words and phrases in posts into hyper-links to, basically, spam and junk web-sites. If you go to your profile->Settings->General settings, all the way at the bottom, you'll find the SkimLinks section. Un-check "Skimlinks enabled".

Regards,
Ray L.