"How to" for the tool table.

[Zadig]

I've managed in Mach to get by without a tool table. Most of my work is a one off nature so setting up tool by tool using the offsets page in Mach has always been sufficient. I am now pulling what few hairs I have left out trying to figure out how to update a tool table. My machine is a knee mill and I have a Haimer taster, I'm looking to be able to raise and lower the knee and set the zero on the Haimer in order to bring all the pre set tools in the tool table into play.

Firstly, is this possible? If it is could someone take the time to talk me through it or point me in the direction of whatever information that might help. Hopefully I won't need chapter and verse, just something that might help it to "click" in my mind. As always, thanks.

Mike

[cncdrive]

You can update the tooltable:

1.) Manually change the values on the screen.
2.) Using the G10 g-code from g-code file or MDI.
3.) Using the Setfield and Validatefield functions via macro or plugin on the appropriate DRO numbers which hold the tool data.

[Zadig]

Thanks for the reply. Apologies for not making myself clear, it's not the populating of the tool table I am having problems with, it is how to find the offsets using the Haimer and tools so I can populate the table. Again, this may not make sense, but an example of what I have tried is:

Home the Z axis
Put the Haimer in the spindle
M6 T1 G43 H1
Zero the Haimer on the workpiece
Note in the tool table #1 the machine offset for the Haimer
Change tool
M6 T2 G43 H2
Zero Tool to workpiece
Note in tool table Machine offset for #2 T2

I've done this and other ways to determine the offsets but I am still unable to derive the proper system for doing so.

Cheers,

Mike

[andrewbishop66]

I also have a similar problem which for me is not really a problem

same thing knee mill which sometimes during a process I might move the knee my previous solution was Gerrys screen set with a fixed tool height setter on the table normally round about stock hight and an electrical probe in the spindle to set the difference between stock height and tool setter and on each tool change the machine checks the tool hight on the tool setter and adjusts according as the reference is fixed to the table and moves with the knee

I too have now switched to a haimer so have the same issues but as I'm doing a bit of an upgrade at the moment I just check the tools hight manually but I am going to have a word with Gerry at some time to see if the offset can be entered manually but still use the tool hight setter

Don't think I've helped you but I feel better

Thanks, Andrew

[Zadig]

Thanks Andrew for the reply. After quite a few hours of trying to get my head around things, I managed this morning to have a bit of an epiphany. So much so I now have it figured out so I can set up the tool table with the necessary tool offsets and place the knee or workpiece wherever it is required using the work offsets, touch off with the Haimer and launch the program. If any of this sounds like it might be helpful to you or anyone else for that matter, just ask.

[andrewbishop66]

Any chance of a few screenshots of the tool table to give me a few ideas to set up mine

Thanks Andrew

[Zadig]

I'm not sure how much use a screenshot would be. It would only show three or four test entries I used when trying to determine how it works. I'll post here a brief description of what I have found to work for me and if you need any further information I'll be more than happy to share it. The way I will describe here sets up the tool offset entries and allows for a Haimer to Zero the work co-ordinates irrespective of the knee height or part location.

Firstly to set up the tool offsets in the offsets page, it is necessary to place the Haimer in the spindle and home the Z axis. In order to keep the offsets as a direct comparison with the Haimer, I have used Tool #1 in the tool table as the offset for the Haimer and maintained it as 0.000 in the tool length column. When Tool #2, Tool #3, Tool #4 etc. are now entered, the exact offset of each tool is represented with respect to the Haimer reference.

Using the Machine coordinates DRO, starting at 0.0000 position, bring the Haimer down to a suitable reference surface, I.e the table, slip gauge or what I use, a 123 block. Zero the Z axis WCS DRO, followed by G53 Z0 to return to the 0.000 machine home position. Do not zero the WCS DRO again until after all the offsets have been measured.

Place the next tool into the spindle and bring down to the reference surface. Note the WCS DRO, this is the offset between the Haimer and the tool you are now determining. Enter the WCS DRO value into the relevant tool offset location in the tool offsets page. It will be a -ve or a +ve number depending on whether it is longer or shorter than the reference Haimer (I'm sure there will be conventions for this, but for me it is sufficient).

Using G53 Z0 return the spindle to the machine 0.000 position. Install the next tool in the spindle and bring down to the reference surface. Again note the value and place in the appropriate row in the offsets page.

Repeat this process for as many times as is necessary for the tools you have.

Fresh tools can be added with this method at any time as long as the Haimer is first referenced and subsequent offsets measured from it. The offsets do not change if the the knee has been moved between setup operations with this process.

To use the offsets it is necessary to set up the relevant WCS for the part, G54, G55 etc. Using T1 M6 followed by G43 H1 to set up Tool#1 and it's appropriate offset (0.0000) bring down the Haimer and zero it onto the part to be machined. Zero the WCS Z axis DRO.

To check that all offsets are correct, place a tool in the spindle e.g Tool #4 and at the MDI, enter T4 M6 and G43 H4. This will allocate the correct offset from the offsets page to Tool #4. Bring the tool down to a known position above the workpiece and measure to make sure it is correct. The Work Offsets menu page gives a good numeric representation as to what is happening.

The part is now ready to be machined with all the offsets set. As each tool change occurs, the relevant G43 (and offset) H# number will be chosen either by the CAM posted G code or by the operator at the MDI.

I hope I have written this up well enough, I am away from my machine at the moment and working from memory.

Mike

[andrewbishop66]

Hi Mike

Thanks for the explanation It made sense to me so when i get a free hour will give it a try

Thanks Andrew