Haas ST10 Tool and Work offset setting Review

Hey G · Jul 29, 2017

Need a little help...I am setting up a guide for my students and I am creating this hand out. I will have three students on each machine and I wrote this so they don't have to touch off every tool when they put a new part in. I will have each student assigned their own offset...G54,G55,G56. So they can get on the machine and establish the Z face and go. I have about 6 years haas lathe experience, just want to make sure this hand out is making sense...at home on a Saturday. Also, these machines do not have the pre-setter...these are budget friendly school models...lol. Your feedback is greatly appreciated!

HAAS LATHE TOOL TOUCH OFF
- Press “HOME G28”, then perform tool change to needed tool.
- Move tool toward chuck face and touch off on metal shim.
- Ensure the Tool Offset page is active, and cursor is in the active tool geometry column and Press “Z FACE MESUR”
- Then enter the compensation amount of your metal shim…e.g. “-.005” Press “WRITE/ENTER”
- Now your Tool offset Z is set
*Center Cutting Tool- If you are setting up a drill (or any center cutting tool) press the F2 button on the X column, to set X. This sets the X for any center cutting tool.
*Turning Tools- Now move to the OD of the part and make a light cut to true-up the part.
- Without moving the X, press the “X DIA MESUR” button, then type in your actual diameter of the part.
- These steps will be the initial set-up for each tool. Next we will set G54.

HAAS LATHE G54 WORKPIECE OFFSET
- Perform these steps when changing a workpiece to establish new Z0.
- Clamp new part in the chuck.
- Use any previously set tool, move toward the part, and take a light cut to clean-up the face.
- On the control, move your cursor to the Z column on the G54 work offset page…ensure you are on the work offset page!
- Press “Z FACE MESUR” to set new G54 Z0 position.
- Ensure that the X column on this page remains at ZERO!
- Now you can run your part.

Thanks for looking this over for me.

G

Mr.E · Aug 3, 2017

You may want to make an additional line.
After you have established your "Z" offset and did the first part you may want to change the length slightly.
Cursor to your G54 or the one each is using and key in the value to increase or shorten (-.002 or .002) then press "Enter", NOT F1

SeymourDumore · Aug 3, 2017

G

I don't see much wrong with your write-up.
One suggestion - if I may ....

When picking up the tool to a shim, I would take out the "-.005 for the shim" step.
Here is why:
First, in the grand scheme of things, it is not necessary. As long as ALL tools are picked up to the very SAME shim on the chuck, the "fixed" reference
is just that.
Second, it is very easy for the guys or girls to forget the added step of deducting the shim's thickness.

Now, as a contrary view to what I've just said:
Leaving the extra step there allows one to use the .005 shim for some tools, and perhaps say a 2" gage block for others (those which may not reach the chuck)
and still arrive at the correct TLO as long as the appropriate shim (gage) length is deducted.

I for one tell the guys here to touch off on the shim or block and call it good, ( lathe and mill) only to make it simpler with less steps.

Hey G · Aug 3, 2017

SeymourDumore said:
G

I don't see much wrong with your write-up.
One suggestion - if I may ....

When picking up the tool to a shim, I would take out the "-.005 for the shim" step.
Here is why:
First, in the grand scheme of things, it is not necessary. As long as ALL tools are picked up to the very SAME shim on the chuck, the "fixed" reference
is just that.
Second, it is very easy for the guys or girls to forget the added step of deducting the shim's thickness.

Now, as a contrary view to what I've just said:
Leaving the extra step there allows one to use the .005 shim for some tools, and perhaps say a 2" gage block for others (those which may not reach the chuck)
and still arrive at the correct TLO as long as the appropriate shim (gage) length is deducted.

I for one tell the guys here to touch off on the shim or block and call it good, ( lathe and mill) only to make it simpler with less steps.

Thanks for the input, and that makes sense.

I want them to input the shim thickness because it follows the mill method we use. I taught them to set-up the mills the same way with a 1-2-3 block, and to add the 1-2 or 3 inch to the touch off, on the table. So they are familiar with it.

Thanks again for all input guys.

G

YdnaD · Aug 5, 2017

We use half-inch blocks for setting tools on both mill and lathe (and 123 blocks to verify the offsets, but a 123 block would work for setting too). I'd be curious as to why you prefer using a tiny shim, if you have a particular reason behind it. I don't like using shim stock or paper on anything because the students forget to change the jog resolution then happily jam the tool into the workpiece, mill or lathe. Depending on the skill level on display (aka, "there's a bunch of donut head kids that are 10 seconds away from destroying things") we might even swap out the steel gauge blocks with crappy plastic blocks to further protect the students from themselves. Obviously using a plastic gauge block is a terrible idea for machining, but it literally saves us hundreds of dollars every semester. If they smash the plastic block then the lesson is still learned, without destroying the gauge block and insert. Although like I said we don't always use them, only if the students demonstrate they can be trusted with an actual gauge.

Let's just say I've amassed a "bucket of shame" filled with annihilated blocks...lol

How about a verification code for MDI? We have the students run a verification for both X and Z before cutting.
G0 G40 G53 X0.0 Z0.0 T101
G1 G54 G98 X1.0 Z3.0 F40.0 (use different X and Z value depending on where you want the tool to be visually checked with 123 block)

If the code is to be ran on a larger machine then you can add an intermediate line to rapid like 6" away from the workpiece then slowly feed it to the final check position. Whether you need that depends on the size of the machine. We have a couple different models so it has a byproduct of allowing a discussion along the lines of "if only there was a way to speed up the process" while standing at the control.

Be aware that the verification will add a good 5-10 minutes to the machine's setup, depending on how attentive you are. But if you have the time to do it, it's a good practice to help wasting time if something isn't set correctly..

Hey G · Aug 6, 2017

YdnaD said:
We use half-inch blocks for setting tools on both mill and lathe (and 123 blocks to verify the offsets, but a 123 block would work for setting too). I'd be curious as to why you prefer using a tiny shim, if you have a particular reason behind it. I don't like using shim stock or paper on anything because the students forget to change the jog resolution then happily jam the tool into the workpiece, mill or lathe. Depending on the skill level on display (aka, "there's a bunch of donut head kids that are 10 seconds away from destroying things") we might even swap out the steel gauge blocks with crappy plastic blocks to further protect the students from themselves. Obviously using a plastic gauge block is a terrible idea for machining, but it literally saves us hundreds of dollars every semester. If they smash the plastic block then the lesson is still learned, without destroying the gauge block and insert. Although like I said we don't always use them, only if the students demonstrate they can be trusted with an actual gauge.

Let's just say I've amassed a "bucket of shame" filled with annihilated blocks...lol

How about a verification code for MDI? We have the students run a verification for both X and Z before cutting.
G0 G40 G53 X0.0 Z0.0 T101
G1 G54 G98 X1.0 Z3.0 F40.0 (use different X and Z value depending on where you want the tool to be visually checked with 123 block)

If the code is to be ran on a larger machine then you can add an intermediate line to rapid like 6" away from the workpiece then slowly feed it to the final check position. Whether you need that depends on the size of the machine. We have a couple different models so it has a byproduct of allowing a discussion along the lines of "if only there was a way to speed up the process" while standing at the control.

Be aware that the verification will add a good 5-10 minutes to the machine's setup, depending on how attentive you are. But if you have the time to do it, it's a good practice to help wasting time if something isn't set correctly..

I like using the shim on the lathe because it's lighter than the blocks. Also, for the most part, by the time we get on lathes the students have figured out the jog handle pretty well and don't smash anything...but it still happens.

Thanks for your input, I like the idea of using a small .5" block on the lathe...it would be smaller and easier to handle.

On the lathe, we verify using- G0 G54 X(dia. of work); Txxx Z1.; M30...with 5% rapid set. Then we will use a 1-2-3 to check Z distance.

Thanks,
G

Search

Largest Manufacturing Technology Community on the Web

Search

Haas ST10 Tool and Work offset setting Review

Hey G

Plastic

Mr.E

Aluminum

SeymourDumore

Diamond

Hey G

Plastic

YdnaD

Aluminum

Hey G

Plastic

Similar threads