[sjanson]

First let me say that I am a new user, that should explain most of my problem.

Yesterday I was running numerous programs with no issues. Then as I was loading a new program I started to question my toolpath that was generated. So, I went back to my CAM software, regenerated my toolpath. When I reloaded it and tried to graph the project on the HAAS screen I recieved an alert that said, "X over travel range" . Then I tried to load and graph my other programs that I have been running and they all did the same thing.

Now, after working on this for a while I decided to put a negative sign in front of the first X and Y locations on the program. When I tried to graph, it when past those points and then errored on the next positive X & Y. It seems like somehow I screwed up my coordinate system. I have pressed many buttons in between all of this.

Can someone tell me what I did wrong.

Thanks,
Scott

[Malish]

I get this allot when loading a new program. One thing you got to watch out for is your tool and work offsets.

If your using tool/work offsets (G54, G55...ect) you can put yourself outside ot limits of travel very easy. If the last part you ran was large or positioned off center on the table you might have probelms if you dont set it up for your next peice before running the simulation.

I also had problems where the last tool that was in the holder was very long (like a drill would be) so the tool offset is set really high and then you do a Z retract move and you get the out of range problem.

[gar]

060623-0936 EST USA

sjanson:

Your problem relates to G5x values inter-related with other values.

Are you close to Ann Arbor?

.

[philholt]

I would check limit switches and make sure there are no chips lodged on them. On my Mini Mill I had a proble similar to this and thought I had really screwed things up. I call a Haas service guy and he told me to check the X limit switch and when I did I found that I had a chip sitting right on top of the limit switch. This may not be what is causing your problem, but it is a place to start. Sometimes a problem that looks complicated and expensive is really simple and cheap.

[sjanson]

Gar,
Not really close to Ann Arbor, I am in Troy which is about an hour away from Ann Arbor

[gar]

060623-1017 EST USA

sjanson:

HAAS defaults on power up to G54 as the base coordinate system on newer machines, meaning maybe after mid 90s.

There are three modes on HAAS mills --- HAAS, Fanuc, Yasnac. Only Fanuc and Yasnac on lathes. HAAS and Fanuc are similar. Fanuc forces G52 to all zeros on power up, program start and some other conditions. In HAAS mode G52 is not changed by these different initialization conditions. In HAAS and Fanuc modes G52 is combined (added but maybe subtracted on some machines) to the current G5x coordinate system.

You need to find out what mode you are operating under. Next determine what G5x is specified in your program, if any. Check the X value of the G5x and see where this puts origin on the table. Make sure all G52 axes are zeroed. Then look in your program and make sure that the first X axis move does not put you off of the table relative to your G5x X axis position.

.

[HuFlungDung]

3 steps to follow:
-load the new program
-set up all the tools and enter the length offsets
-set the first piece of stock up on the table. Use your edge finder to find the location of the stock X0Y0, which you determined by the position of your part on your CAD screen. Teach these coordinates into your control by being on the work offsets page, and pressing the cursor until the correct axis is highlighted across from the correct G5x work coordinate system, and press the "Part Zero Set". Set one axis at a time (this is how it works).

THEN, you are ready to do the graphics mode check. When everything is set up this way, then the graphics mode check will offer a valid check of tool and axis overtravel.

[sjanson]

All,
Thankyou for all of the great suggestions, I did run through them all.

What my issue ended up to be is that when I generated a new code using my CAM software it reset the coordinates for G92. Instead of G92 equalling zero for X & Y it had some values in there. Then when I was asking the machine to go to the part zero, it was putting the table out of range.

I learned a lesson I'll never forget

Thanks again,

Scott

[HuFlungDung]

Scott,

Lose the G92 altogether. It is not needed in normal use and it mucks around with your machine coordinate system.