Machsupport Forum

Mach Discussion => General Mach Discussion => Topic started by: 30t000 on July 11, 2009, 11:53:59 AM

Title: Setting tool offsets
Post by: 30t000 on July 11, 2009, 11:53:59 AM
Hi again everyone,
     I am having a spot of bother trying to set tool offsets . I use fanuc all the time at work and have tried to set the offsets in a similar manner to them without success . I have included a couple of pictures to help give you all an idea on what I am obviously doing wrong .
     The sequence is to home the machine with a 4" slip in both the "X" and the "Z" . The "Z" is set between the chuck face and the edge of the homemade toolplate (101.6). The "X" is set to 203.2 as I am in Dia mode . I then set the "Part X Zero" to zero and do the same with "Part Z Zero". I do not seem to have a problem setting the "Z" offsets , but the "X" is really getting to me now .
     The machine is using a rear tool post as can be seen with the spindle running clockwise looking towards the tailstock and the insert upside down . If I move the drill (tool n°2) in to "X" zero after setting the offset , the part DRO does not also correspond to "X" zero . The same happens with the turning tool . To my mind , the "X" axis datum should never move .
     So can someone be kind enough to explain in really basic language how to set the offsets please . The screens are all as standard if that helps .
Title: Re: Setting tool offsets
Post by: Hood on July 11, 2009, 04:09:19 PM
Set a home off value for your master tools X  and dont have any  offsets for it in the tooltable. All the rest of the tools are then set up to that tool by entering the values in the tooltable.
Title: Re: Setting tool offsets
Post by: jimpinder on July 13, 2009, 03:33:34 AM
If you have a tool that you use more often than others, then use that. Other than that  you can use any pointer, or a marker that you wish. It need not be a tool as such.

When setting up my tool table, I used a corner of my cross slide as the marker, because it was easy to measure to and from, to the tips of the tools I put in the holder.

Set your homing with, as Hood says, offset positions, so that when you home the machine, your marker/pointer or tool 0, (whichever you are using) homes to position 0,0 i.e. I assume X0 is on the centreline, I have my Z0 on the chuck. The DRO's should all zero (machine co-ordinates)

Now place the tools in their relevant holder - and it does not need to be all the same holder - and measure with a set of digital calipers, the distance from your marker to the tool tip. This is your tool offset. You can move the table to a more convenient position to do this.

You can test the offsets by putting the tools in, and (as I am sure you know) typing in the tool number, bearing in mind for Mach Turn the Tool number is a four figure number eg. T0202 - (tool number 2 and offset 2) both pairs of numbers must be included. G0X0Z0 should then take the tool tip to your 0.0 position.

You can see why I use a seperate marker. In my case, the corner of the cross slide is always there and I can always measure to it, especially if the tool is one you do not use all that often, and you wish to check the offsets. If you use a tool in a holder as a marker, you have a lot more adding and subtracting to do to get the differences in length and position.

Like you I also have a centre drill holder at the back of the table. I have made holders for all my drills so they just slot into it to a set depth. X offset is always the same, of course, and the z offset brings then point of the drill to the centre of the chuck, just in the little space between the jaws. This makes any depths easy to calculate.

Title: Re: Setting tool offsets
Post by: 30t000 on July 13, 2009, 12:47:42 PM
Once again I find the answers coming freely . Thanks again Hood and also thank you Jim (I presume) . Unfortunately I find the tool screen is full of information and buttons that do not (seems to me) make life easy . I think the designers have tried to cater for all possibilities and in doing so have messed with my simple head . Not complaining , but sometimes more can be less .
I think I got it covered using the turning and facing tool as a reference and then setting the other tools to that tool as suggested by Hood . The problem I foresee is if you take away the tool and replace it with something else . Then I would have to set all the tools again relative to that one . I would like it where I set the tools up once relative to something ???????? and then it will not matter what tool is changed . The tool library can then stay the same no matter what facing turning tool I use . If that makes sense .
Title: Re: Setting tool offsets
Post by: Hood on July 13, 2009, 05:23:10 PM
 I am almost certain that when you restart Turn it is offset 1 that is selected so that really should mean you have  no offset in the tooltable for offset 1. Notice I am saying offset rather than tool, this is because with a lathe you usually have tool slots in a turret or toolpost and using the T0101 you are calling Tool 1 and Offset 1, it is quite possible that you will have other tools that you can put in these slots and thus just call the same Tool number but a different offset, another thing is the ToolTable is not actually a tool table it is a Tool Offset table.
 So to answer your question, you could quite eaily treat your home position as your Offset 1 position and then set all tools up from there, just have to make sure that offset 1 is never used by a tool so you could do two things, firstly never call Tool 1 or if you want to use Tool 1 then make sure you never use Offset 1 with it.

Hope you understand as I know what I am trying to say but its hard to put in words.

As for the Turn screen, well I have never really used it, just looked at it and didnt like what I saw so I adapted my Mill screen to suit. One day I will get round to actually making it a proper turn screen but for now it does fine :)
Title: Re: Setting tool offsets
Post by: jimpinder on July 14, 2009, 02:45:16 AM
I also find the tool offset page  too ***. My apologies to whoever designed it.

Yes - your point about changing tools and loosing the relative position is what I was trying to say. You can make your reference point anything, as Hood said.

This is why I use the corner of my cross slide - that never gets taken off the lathe, and is always there to measure to. When you "Home" the lathe, set the "home offsets" on the homing page, so that if you then put in a command G0X0Z0 the table moves so that the corner of the slide is in position X0 Z0. As I say, mine 00 is touching the chuck (Z0) on the centreline of the lathe (X0).

I now set all my tools in the holder and measure their position relative to the front corner of the cross slide. Job done. If I change tools or fittings on the cross slide, the corner of the slide is still there to measure the new tool to.
Title: Re: Setting tool offsets
Post by: 30t000 on July 14, 2009, 01:20:17 PM
When I use the mills at work (CNC of course) , tool 1 is the probe and all tool lengths are set to that . Where as the the lathes are set to a defined point on the machine . Both work , but being a turner predominantly , I prefer the latter . I will give both a try and see what happens .

 Thank you to the pair of you .