[FFWD]

Hey guys. I can't seem to figure why my Fadal 4020 doesn't like this.

Just before the machine hits a tool change line, it will want to crash into the floor instead of rising to the ATC.

It had run fine before using Featurecam 2013.

The only difference I have made is I converted over to using the actual tool lengths for my H numbers (H1-H21), for simplicity sake, along with using a fixture offset number. You know...taking the tool length and adding that from the Z number given when the spindle itself is sitting right on top of the stock. The difference is my Z0 for that particular tool...nothing uncommon.

Code where it hangs up:

N235G0Z1.12
N240G0Z0H0M5M9
N245* T 2 DIA 0.75
N250T2M6 * 3/4" E.M.

This excerpt is placed at the end of the first op...going to do a tool change.

I've tried removing the "H0", adding a G53, as well as taking the Z0 out. It did solve the problem of the head plunging, but now that basically makes the head go up PAST machine home...to the point of giving me a nice amplifier fault.

Any ideas on what is going on here? Is there something that needs to be cancelled in the code for some reason now? Why problematic now instead of before when it hit the end of a op and tool changed smooth as silk. FYI...it currently operates the first op just fine with that tool. Z is exactly where it's supposed to be.

Something to do with changing my offset inputting between the tool and fixture perhaps?

The 1990 4020 has the basic CNC88 controller running Format II. Always has with no issue...even back in the "write each line of code" days.

Thanks for the input guys!

[txcncman]

Try G0 G28 G91 Z0 before M6 line.

[jeffn]

if i am understanding this right your fixture offset is your spindle sitting on the part. the G0 H0 Z0 wants to cancel out your tool offset and send the spindle to the top of the part because your fixture offset is still intact. your tool is in between the two of them, though.

a G53 without the H0 Z0 is cancelling out your fixture offset but leaves your tool offset intact which i am guessing is a positive number. if it is greater than 4" your machine is gonna fault out.

personally i wouldn't put a Z in my fixture offset but if you are gonna, i am guessing that line should have a G53 along with the H0 Z0 so it cancels out both the fixture offset and tool offset, sending the Z axis to it's home position.

[FFWD]

Interesting input guys. I appreciate that!

Actually, I kept dorking with it and got it to work with a simple line addition.

First, I merely removed G0Z0H0, inserted a G28 line right after the M5M9 line everywhere in the program there was a toolchange, and I was golden. The H0, the machine REALLY didn't like...which sent it plunging to China every time.

Now, it took lots of educated guesses/combinations (some of them as recommended above), but I nailed it at least.

Interestingly enough, at the very end of the program, that was a different story to send the head back home. It took a G53 in addition to the G28 in order for it to work correctly. Hmm...



From you are saying, I didn't notice it before when I had used the other method of offsetting because my tool offset previously was very minimal if anything at all. If the head dropped, I never noticed it. It certainly wasn't going to cause a problem if my tool offset got cancelled.

Although the machine crashed, at least I figured out on what it likes to eat and mod the code to suit. Although a rocky start, I still like the idea of setting tool lengths with my setter and fixture offsets with the spindle on the stock because of running about a 7 fixture setup....the same tool does many jobs on more than one fixture plus the easier numbering scheme (and not using a ton) of my H numbers.

Again, thanks a bunch for you guys' input on this! :cheers:

Do any of you guys know if there anything in post (or anywhere else for that matter) I can do with Featurecam to apply these workarounds I applied in the code?

[cadman]

G53 is the machine coordinate system, and is non-modal. Line N240 should be:

N240G53Z0

You need the axis you are going to on the same line. If you want M5M9 on the same line, that is your option. You don't need to cancel the tool offset on the way to the tool change, but obviously need to pick up the correct tool length register on the way down.

YMMV, but the only place my Fadal posts cancel the tool length is at the end of the program:

NxxxM5M9
NxxxG53Z0
NxxxTxxM6
NxxxX0Y0Z0E0H0
NxxxM30

IMO, cancelling the tool length somewhere in the body of the program is potentially risky if you have operators, and I've seen the results at every shop I've set foot in.

I don't use FeatureCam, so I can't help you there.

[Superman]

Here is a link for good reading,
- on how to make the machine return to it's home position
using various methods

LINK

[FFWD]

G53 is the machine coordinate system, and is non-modal. Line N240 should be:

N240G53Z0

You need the axis you are going to on the same line. If you want M5M9 on the same line, that is your option. You don't need to cancel the tool offset on the way to the tool change, but obviously need to pick up the correct tool length register on the way down.

YMMV, but the only place my Fadal posts cancel the tool length is at the end of the program:

NxxxM5M9
NxxxG53Z0
NxxxTxxM6
NxxxX0Y0Z0E0H0
NxxxM30

IMO, cancelling the tool length somewhere in the body of the program is potentially risky if you have operators, and I've seen the results at every shop I've set foot in.

I don't use FeatureCam, so I can't help you there.

Interesting! It sounds like I was being redundant in my modification to get this machine not to crash and/or return to home. Although it is working right now, cadman, what do you suggest I mod each section of the program to just before the tool change line? I want to start off with a good practice in my workflow.

Take the line I had placed my G28 code and merely replace with G53ZO? That will not cancel out any tool offsets but send it to home for the tool change?

For example and clarification, every time there is a tool change, Featurecam writes:

NxxxG0Z1.03
NxxxG0Z0H0M5M9
Nxxx* T 2 DIA 0.75
NxxxT2M6 * xxx tool

At the end of the program, Featurecam puts:

NxxxZ1.03
NxxxM5M9
NxxxG0Z0H0
NxxxX0Y0E0
NxxxM2

What do you suggest to modify these sections to (which will tell me what I have to do every time I spit out a program in Featurecam)? Just to make sure I'm understanding your method/practice here.

BTW, great link buddy! Easy to forget this stuff.

[txcncman]

Here is a proven working Fadal program for your reference. Note machine is always started with Z at the home position and programmed to return to Z home after each tool process.

[FFWD]

Appreciate all the help guys! This is certainly a nice forum to be in.

I'll give those ideas a whirl for future work and reference the uploaded program.

Chalk it up as another learning experience! :cheers: I never would have thunk it...

[Joe S.]

What do you suggest to modify these sections to (which will tell me what I have to do every time I spit out a program in Featurecam)? Just to make sure I'm understanding your method/practice here.

BTW, great link buddy! Easy to forget this stuff.

My Fadal likes G91 G0 G28 Z0 to send the spindle home with no H or G53 , in fact My Fadal doesn't accept G53 G54 ... it uses E1 E2 as offsets

[Geof]

We're not in business to make parts, we're in business to make money, making parts is just how we do that.

I like this. So many people on this site who run machines seem to forget the primary reason for running a machine.

[Joe S.]

We're not in business to make parts, we're in business to make money, making parts is just how we do that.

I like this. So many people on this site who run machines seem to forget the primary reason for running a machine.

Thanks Geof, I WAS thinking about changing it but will keep it now a while longer, I like your avatar too, too many have allowed that leakage.