[Captdave]

Hi Guys been awhile since I posted. I'm starting to change the way I have been setting tool lengths since I"m using the VM-10 for more then just second op work.

I had been setting the tools off the top of the part and measuring each tool as I go but that is getting old fast as the jobs I'm running now require 5-10 tools each.

I have a conversational program Called "tools" that I keep all the tool data in and import it into the program I'm working from.

What I have done is gone back thru all the tools and reset them off the table with a touch off gauge to set the tool length and saved the "tools" file. Imported the "tools" file into the working program and using the same touch off gauge set the part off set in the working program.

All was well until I went back an touched off another tool into the "tools" file, saved it and imported it into the working file and the tool took a dive well below the programmed Z0.

What did I miss? Do you have to zero out the part offset prior to importing tools?

[fasto]

All was well until I went back an touched off another tool into the "tools" file, saved it and imported it into the working file and the tool took a dive well below the programmed Z0.

What did I miss? Do you have to zero out the part offset prior to importing tools?

I don't have Winmax (wish I did...), on Ultimax you do need to zero the part Z offset or it gets added to (subtracted from) the tool zero depending on its sign.

[Captdave]

This is the first CNC mill I have used but I have to wonder is it common to all control types to have to zero the work offset prior to calling a new tool? Is it a hurcoism due to having tool offsets stored in separate file.

[fasto]

This is the first CNC mill I have used but I have to wonder is it common to all control types to have to zero the work offset prior to calling a new tool? Is it a hurcoism due to having tool offsets stored in separate file.

You don't need to zero the work offset before changing tools if you're talking about toolchanges during the program execution. This assumes your tools are all zeroed at the same point, etc. The work offset should shift the Z zero of all tools equally. In Gcode you'd call a new tool offset when you called for the toolchange, in Hurco Conversational that's automatically done for you - don't know about Hurco Gcode.

If you replace a tool and have to touch off again, you do need to zero the work offset because the work offset is, well, offsetting the zero you're touching off against. You can also touch off your usual spot and then subtract the work offset from the resulting tool zero which has the same effect (and is pretty easy even on Ultimax). I remember this being explained in the Ultimax programming manual.

As I understand it, the "professional" way to handle this is to use a tool presetter to adjust your replacement tool to the same gauge length (which gives the same tool zero as your broken tool). Of course, you need to buy or make a tool presetter - item # 3,886 on my to do list. On machines with a tool probe it sets the tool offset for you. Presumably it handles the work offset issue automatically somehow - I haven't got a tool probe.

There are lots more ways to handle this. I don't pretend to know them all.

[pgf545]

Go into the program paramaters and change the add tool offset parameter to no and that should take care of your problem. I set my tools off the table using the touch off probe and then touch one tool to the "Z" on the part and I don't have any problems. Then if you break a tool all you have to do is retouch the tool with the probe off the table again and you will be good.

Bernie

[Captdave]

Go into the program parameters and change the add tool offset parameter to no and that should take care of your problem. I set my tools off the table using the touch off probe and then touch one tool to the "Z" on the part and I don't have any problems. Then if you break a tool all you have to do is retouch the tool with the probe off the table again and you will be good.

Bernie

Here is what I found in the WinMax manual:

• Include Offset Z in Tool Zero Cal—Indicates whether or not the Offset Z
value in Part Setup is added to the zero calibration value when tool lengths
are adjusted. Default is Yes.

Just to make sure I've got my head around this. Change the Z offset value in the parameter to NO. If resetting a tool it must be in the "tool" file, save the file then import it into the working part file. Then no changes are required to the part Z work offset?

[pgf545]

Here is what I found in the WinMax manual:

• Include Offset Z in Tool Zero Cal—Indicates whether or not the Offset Z
value in Part Setup is added to the zero calibration value when tool lengths
are adjusted. Default is Yes.

Just to make sure I've got my head around this. Change the Z offset value in the parameter to NO. If resetting a tool it must be in the "tool" file, save the file then import it into the working part file. Then no changes are required to the part Z work offset?

Ok I am running the Ultimax on my machine but ran a Winmax machine at another shop a while back. If I remember right it set up the same. Also I think the Winmax stores the tool setup seperate from the program but it has been a while. You don't necessarily need to store it in the tool program, you can store it in the part program but you will need to import that information back into the tool program after you are done to make sure it gets stored properly for the next program. I think you are on the right track and I am terrible at trying to explain things in writing...lol. Hope this helps and if not I will give it another try.

Bernie

[Captdave]

I'm running a rather long job now but will give it a try on the next setup.

Thanks Bernie.

[glovebox20]

[QUOTE=Captdave;952946]Here is what I found in the WinMax manual:

• Include Offset Z in Tool Zero Cal—Indicates whether or not the Offset Z
value in Part Setup is added to the zero calibration value when tool lengths
are adjusted. Default is Yes.

QUOTE]

If you are touching off All your tools from a Common Ref. point (like you are describing), I would defenitly would want to change "Include Offset Z in Tool Zero Cal" to NO. This way it dose not matter what Z offset you have in your part set up, it will always store the offset from machine postion.


If "Include Offset Z in Tool Zero Cal" is selected to Yes, than the Z offset in your part setup will be added to the tool offset, witch could be bad in this setup. I would say this may be the problem you had as long ad the Z offset of the part was right and you imported the tool lengths correctly. I belive the "Ultimax 3" and eariler controls did not have this parameter.

glovebox20

[Captdave]

I would defenitly would want to change "Include Offset Z in Tool Zero Cal" to NO.

Works like a champ! Thanks for the tip.