Haas and HSMWorks tool offset

Hello,

I have just purchased a Haas mini mill 2006, and I have a problem understanding tool length. The problem is that I shall make measures in my HSMWorks tools directory, and also on Haas machine in the tool offset settings. (Picture in attachment. )

What happens then? Does the tool length is doubled as it is defined in HSMworks and in Haas tool lenght settings, or it will behave normaly.

For example, if I take a measure for the one random tool which I will use on my work piece (G54), will others toolss be also adjusted to the work piece.

Newbie here, so be gentle.

Thank you

Marko

It definitely shouldn't be doubling the tool lengths. Don't use the software tool lengths if it's going to do that.

https://youtu.be/uNjMIIRttFE

Thank you fellas for quick reply.

I have gone trough the whole videos before asking the questions, and after a day of testing some offsets, I have answered to my questions.

Now, most of the machinist are making simple G-codes by hand, and I need to make them in HSMWorks, which makes all the problems to float. For example, If I define my own bits setup(length , offset, diameter), than machine bits settings should all be Zero, and then my program works. If they are defined on a machine, and on a CAD/CAM software, then there will be an error, or a crash, beacuse if for example: Tool 1 has offset of 100mm, and in my machine also is defined an offset of 100 mm, the machine will take both offsets and will plunge 200mm in -Z direction, which will result in alarm, error or a crash.

I have defined them all by hand in the machine, and this is only for reasons that if you want to make Gcode by hand on the machine, or in some editor. This settings should be zeroed (All tools measures shouled be set to 0) if you are using a CAD/CAM for generating Gcode.

Cheers,

Marko

I recommend you do not use length offset in HSMWorks. Ever. I don't even know how that works in the G code. H is always set at the machine. What if a tool has to be changed? No. Always at the machine for length. IMO

Diameter is a different matter. Tell the machinists to set their Diameters to zero. Then offset as needed.

Totally agree with above!

Agreed, only at machine.

Hello again,

I dont think we understand each other, so I will try to explain.

In that video you posted, it is shown how to define and "level" all the tools, but I have very short tools, and when I set their offset, it states that my Tool has an offset of 230.xxx mm, which is imposible.

What makes sense is that I should measure my tool holder first, and then mount my tool to to measure it again, because no tool can have that offset, and in that video it does not says what is the actual offset.

If somebody can make sense of it, as I cant, and no tool can have offset of 2xx.xxx mm when its lenght its 30.xx mm

Thank you

Marko

It is whatever you decide it is. What is important is that you are measuring against the same reference you are using to set your Z work offset.

If this doesn't make sense, you _really_ need to get a basic understanding of how this works.

If you are using WIPS, which you haven't said you are, then that system needs to be calibrated.

Quote:

---

Originally Posted by lopata

Hello again,

I dont think we understand each other, so I will try to explain.

In that video you posted, it is shown how to define and "level" all the tools, but I have very short tools, and when I set their offset, it states that my Tool has an offset of 230.xxx mm, which is imposible.

What makes sense is that I should measure my tool holder first, and then mount my tool to to measure it again, because no tool can have that offset, and in that video it does not says what is the actual offset.

If somebody can make sense of it, as I cant, and no tool can have offset of 2xx.xxx mm when its lenght its 30.xx mm

Thank you

Marko

---

Unless I'm misreading something, your 230mm tool would be 9" in imperial length. What is wrong with that? The measured length for offsets is from machine Z0. to the top of the part zero. Nine inches or 230.00mm would be fairly common with many tools. You are not measuring the tool it self. You are measuring the tool tip to the part Z 0..

I suggest you reexamine the touching off with paper part of that video and use that method. You need to get yourself acquainted with the machine before jumping into preset offsets etc. The only error in that video is that after just touching the paper, you need to go .004" or .100 mm farther. If it just touches, .004", if it touches/drags very hard then go .003".

Save yourself a bunches of crashes and use that touch off method for a while.

Thank you for this reply.

I have now understood what was missing the day before. That day the local machinist explained to me that I need to make measure every tool each time I use in on all tools. Could not be further from the truth, I understand it now.

This is my comprehension of the machine. As I set my tools offset, I would not change the tools until I replace them, so once the offset of each tool is defined, I only need 1 tool to touch off the work plate, and then go to second OFFSET tab, and subtract the preset tool offset from machine Z coordinates.

I have done a few tests, and this is the way it should make sense.

It is much easier to keep tool length 0 and asign separate offset for every tool. It will keep your tool setup for every programm and the benefit is that U see the tooltip coordinate Z directly. U can fit it in CAM as well if U like, the only problem is when U need to tilt spindle with keeping tooltip on surface... it will require a modification in post.

Quote:

---

Originally Posted by lopata

Thank you for this reply.

I have now understood what was missing the day before. That day the local machinist explained to me that I need to make measure every tool each time I use in on all tools. Could not be further from the truth, I understand it now.

This is my comprehension of the machine. As I set my tools offset, I would not change the tools until I replace them, so once the offset of each tool is defined, I only need 1 tool to touch off the work plate, and then go to second OFFSET tab, and subtract the preset tool offset from machine Z coordinates.

I have done a few tests, and this is the way it should make sense.

---

No offense, but I feel like giving up! You touch off every tool on every different part you run. Any change in the tool or the part requires a change. The machine has no idea where your part is or where you tool is. It does not know the type of tool, the size of the tool, or the length of the tool, or the location and height of the part. Touching off means you are telling it where everything is. Otherwise if you tell the tool to go to Z0. and that is 100mm lower than you piece of material or the table of your machine, it will go and crash through it. It does not know anything. Touch off the tool any time for a different part. If you are running 100 of the same parts with the same material and size, then touch off once. If you run one part then go to a different job or part then touch off all over again.

Kind of like a GPS system that you tell to go to a specific location, but you don't tell it where you are starting from, it has no idea how to get there from where you are. The machine will do what you command it to, no matter how dumb that is.

@machineit that depends how you do it, but I prefer doing it like he says. I change my work coordinate z and leave the tools the same. That's how you would do it with a renishaw probe system as well.

Hey,

I dont think I follow here. Can you explain in more detail please. I dont understand the part of tilting spindle?
And how to do you get tool lenght 0, on the machine, or the CAM program?

Cheers

In cam U don't bother with tool length, just make postprocessor to call new offset right after toolcall and then setup suficient offset for every tool and reset tool length in tables for 0. It will work for sure even if U will get g43 in programm.

Quote:

---

Originally Posted by Machineit

No offense, but I feel like giving up! You touch off every tool on every different part you run. Any change in the tool or the part requires a change. The machine has no idea where your part is or where you tool is. It does not know the type of tool, the size of the tool, or the length of the tool, or the location and height of the part. Touching off means you are telling it where everything is. Otherwise if you tell the tool to go to Z0. and that is 100mm lower than you piece of material or the table of your machine, it will go and crash through it. It does not know anything. Touch off the tool any time for a different part. If you are running 100 of the same parts with the same material and size, then touch off once. If you run one part then go to a different job or part then touch off all over again.

---

I used to do it that way, and honestly I found that it sucks. If you run large quantities of parts per setup it might not be so bad but if you change setups a lot it means you are always touching off tools. And it's totally unnecessary.

The better method is to always touch off your tools to a fixed reference point that NEVER changes. It doesn't really matter where this point is, it just needs to be constant. When you load a new tool you set it's offset (to the fixed reference) once and it never changes until you take it out of the machine. Now when you setup a job, you set the work offset to the difference between the fixed reference point and the top of the work. The way I do this is to use my spot drill as a sort of probe, since it's always in the machine and never changes. I know that its offset to the fixed tool reference point is 10.675. So I jog it down to the top of the work (starting from machine Z0) and subtract that value from 10.675. The resulting value is your work offset. It may be positive or negative depending on whether the work is higher or lower than the tool reference point, but as long as you keep the sign it doesn't matter.

The nice thing about this method is that if you break a tool in the middle of a job; you just load a new tool, reset it's offset to the fixed tool reference, and keep going. If you set your tool offsets based on the top of a work piece, once you machine off the top of that work piece you've now lost your reference point. Now if you break a too you have to figure out how to recreate that reference point, or set the new tool to some other area of the part with a known distance from the original work zero. If the part has no flat areas to reference you're screwed and have to start over again. Been there. Done that. Don't want to do it again.


C|

My thoughts exactly. Thank you C.

My fixed point of reference is tool height gauge mounted on a stock table, which is always the same height. My tools are fixed, and I wont be changing them until I break them, or they wear off.

I use a lots of setups, or JIGs, and I only want to measure Z0 with tool#1 (which is a sensor probe), which is also fixed and wont be changed, until stated above happens.

When I touch off with Tool#1, I deduct current Z position and my tool#1 offset and I have my setup Z0 set for all the tools.

This is what I needed, and have to run a few more tests to confirm it, but your post and my previous test just proved my theory.

That method will work, it's just an added step when compared to Machineit's description. The advantage of not using the work offset Z-value is that it's simple to understand, but the disadvantage is that moving between different parts requires re-measuring every tool unless your material or Z-origin is identical each time. There's advantages and disadvantages to both methods, either way you'll need to be sure you understand the offsets.

Before running the actual program, you should check the offset values by running a "verification" code using MDI to ensure your TLO values are correct. Check it with a rule or gauge block of known thickness (100mm in the below example). If the tool gets any closer than 100mm, stop the motion and re-check the offsets. Using a big distance is a good idea (3 inch blocks are common in the States, I'm not sure what the common metric equivalent is).
T1 M6
G1 G90 G54 G43 H1 Z100.0 F500.0

You will need to modify the code to suit the tool being checked (T and H must match), whichever work offset is being used, etc.

Quote:

---

Originally Posted by Ydna

That method will work, it's just an added step when compared to Machineit's description.

---

If you always reload every tool every time, then yes, the separate work offset method will add an extra step. But if you reuse just one tool, it's a wash. If you reuse two or more tools, it will reduce the number of steps. That and the easy recovery from broken tools makes it worth doing for me. I rarely break tools, but the first time I did after switching to the separate work Z method, recovery was so fast I was sold.


C|