Question...How do I change my lathe reference tool?

[Reedfirst]

Hello Everyone,

I need to change tool 1 in the CNC Lathe software which is also my reference tool.

Is there a way to change out the reference tool (tool 1) without affecting the other tools and having to re-enter all the offsets?

thanks!

[cnckeith]

change the insert you mean?
you could put in a new reference tool of the same length of the old one. is one solution..
if you use an actual tool at a reference tool..this is a gotcha..so instead use a dedicated reference tool not an actual tool that you are going to cut with so it never changes length then you never have to remeasure all the tools against a new different length reference tool.

[Reedfirst]

I want to change out the entire tool because it uses an insert that i find is a little too large for the Techno lathe (dcgx 32.51). I'm switching it out to a tool that uses the same insert but with a smaller inscribed circle to try and get some stringy chips under control (dcgx 21.51).

I usually make a skim cut with my reference tool (tool 1) on a piece of scrap to set the x coordinate and Z(zero). That way any runout of the chuck is eliminated when setting up. Since there may come a time I'd have to replace the insert in my reference tool (although not for a very long time) I am wondering. Is there a better way to do this?

[Chaz]

Ive got the same issue, I use tool 1 as my reference and if I break that insert or it moves, I'm screwed too. I think what Ill do and what the OP will need to do here too is reference off something else in future.

Perhaps a shortcut would be, before tool 1 breaks, reference off a new method, check the distance differences between current tool 1 and new reference and then simply do some math to calculated the new addition (or subtraction) from the offsets. For example, if the new reference is 2.5mm further on the X, then work out if that needs to be added or subtracted and do that for all the tool offsets. Quick manual or excel job and sorted, same for Z.

[Reedfirst]

I've decided that for now I'm going to dedicate my tool 1 holder and the insert as the reference tool. It's an imported holder so not much money lost in using it for that purpose.

I have however been thinking about a work around for this. Maybe someone can chime in if this is a workable solution or not.

So let's say in my case tool 1 is the reference tool and every other tool in the library is the length difference between x and z. Would it be possible to set the reference position in tool setup for Tool 1 and then somehow tell the software to "swap" reference tools. Lets say from tool 1 to tool 2. Since the offset information is already in the computer for tool 1 and tool 2; Is there a way to have the control apply the offset difference between tool 2 and tool 1, . Make tool 2 the new reference tool and apply the additive or subtractive offsets to the other tools in the library automatically?

I hope what i'm explaining makes sense.

[cnc_smith]

I've decided that for now I'm going to dedicate my tool 1 holder and the insert as the reference tool. It's an imported holder so not much money lost in using it for that purpose.

I have however been thinking about a work around for this. Maybe someone can chime in if this is a workable solution or not.

So let's say in my case tool 1 is the reference tool and every other tool in the library is the length difference between x and z. Would it be possible to set the reference position in tool setup for Tool 1 and then somehow tell the software to "swap" reference tools. Lets say from tool 1 to tool 2. Since the offset information is already in the computer for tool 1 and tool 2; Is there a way to have the control apply the offset difference between tool 2 and tool 1, . Make tool 2 the new reference tool and apply the additive or subtractive offsets to the other tools in the library automatically?

I hope what i'm explaining makes sense.

I have run into the situation where my reference tool has changed because of changing inserts. In my case the reference tool is my roughing tool and I keep the X and Z offset both at 0.0 For adjusting the difference I use the Wear Offset to get it to cut to the right size. With parameter 3 set to a 4 (which is the default) when you go into the Tool Library the tool that you have called up with the offset on is the active tool. With the lathe you can use any tool that has had the X and Z offset set be used to set the X Dia and Z Ref. The first time setting up the tools you need to have a Reference tool. Once the other tools are set you can use any tool that has been qualified (my wording for tools that have had the X and Z offset set). You highlight the tool that you are using to set Z Reference and use that tool to set Z reference. The same for X Dia. With over time I might get difference values set in my Tool Wear Adjustment. At some point I will want it to have 0.0 in for the X and Z Tool Wear Adjustment. I will write down the values and set the reference tool Tool Wear Adjustment to 0.0. Then I will add or subtract the values from the other tools in the Tool Library by that amount. Both of my lathes have 8 station ATC so I am only using 8 tool stations. So some of the tools are not changed out where several of the stations are being used with different tools so the offset are changing on them so those tools have to be remeasured.

The question of make Tool 2 the new reference tool as I stated above on the lathe once any tool is qualified you can use any of those tools to set X Dia or Z Ref. This is one of the things that is different from the mill.

I hope I did not make this to confusing. The lathe does have differences from the mill in tool setup. The other major difference is setting Z Reference and X Dia. On the lathe if you forgot to set say the X diameter with the Reference tool you can type the know diameter in the "Establish the X Diameter" screen in the Tool Measure screen and set it afterwards. The same is true for Z Reference. As a note make sure the Entry mode: is set to absolute other wise if it is set to incremental it will add the value to the X Dia or the Z Ref.