What's new
What's new

Struggling with Probing

The advantage with G54 is that it is also the default (on Fanuc, and possibly on other controls also). So. if you forget to explicitly command it in the beginning of the program, the program would still run as intended.
From what I have seen thus far, it is the same for Fagor.
 
It's really hard to say anything for sure without seeing and knowing what your system looks like. In your original post it seemed like your numbers where being affected by your early entry of the workpiece height into the G54 Z register. Let's just say that my comment was to suggest that anytime you start a new work height measurement, zero out G54 Z before entering the new. one. I don't even know if your probe automatically enters the number for you like it would on a standard CNC machine, or if it only stops the machine and you read a number off the screen and enter it manually. All these differences and unknowns sort of affect the comments a person can give.
I can say for sure that the probe can and does enter the G54 offset if I use a probing program that I wrote for this specifically for the material top Z 0. Alternatively, I use
very short probing program for the touch off of the top of the hard block which does not set any offset at all. I think the best next step is to do what has been suggested with MDI G54 Z1 and see if a tool that has already been set to height of the block/tool setter is in fact 1" above the work piece. I didn't think to do this and spent way too much time trying to digest the numbers which make no sense to me.
 
I would like to touch on a few things that others have mentioned and add a bit more.

1.) Tools that are fixed in holders should not change in length unless you remove the cutter from the holder. (Yes, tool wear is different, but lets forget about that for now.)

Lets say I set up a 1/4" end mill in an ER16 holder. I will call that tool #2, touch it off and enter it's length on the tool offset page - let's call it + 3.000".

Now, I set up a different job on the mill that requires me to crank the table down to an unknown distance - as long as I have not removed that end mill from that ER16 holder - I will be able to run that tool again in my new program without resetting it's length.

2.) Building on the information above; the length of your material touch probe never changes; unless you physically change it by replacing the stylus. Setting the probe length is technically a calibration; once it's length is known, do not change it.

3.) Your tool length offsets should be positive numbers; they should reflect the actual, physical gauge length of each tool.

4.) Because the knee moves up and down, the actual distance from Z home, to the tool setter, will change frequently. This is the number that you will want to update each time you move the knee.

Each time the knee is moved for a new job, begin by probing that block like you were doing but, instead of updating the probe length; you will update the distance from z home to the tool setter trigger point.

Does this make sense?

Where does your machine store the offset location data for that tool setter?

We can cover how to find the actual gauge length of the probe next.
#1) I understand and agree with the first two sentences. The 3rd sentence had me a bit confused, but as I read it the second time, I think it too makes sense since the delta in height is compensated by the G54 (or other) offset, is that right?

#2) does make sense now that I see it in words and digested it. Why would it change, it is a physical distance that is constant unless the tip brakes, etc
#3) Having a hard time with this statement, or maybe don't understand it. If the material probe (tool #1) is 3" long and and the first tool (tool #2) is a 1/4" end mill with an OAL of 2" and part of it is in the holder, I get it being a positive number, but what about T-4, a 1/2 drill that is 5" long? Wouldnt that be a negative number?

#4) Understood

Your next sentence for me is one and the same. The block that I made I surface ground to within a couple of tenths of the trip point of the tool setter so probing with the material probe to the block is more or less identical to a tool touch off to the tool setter.

The offset location of the for the tool setter is the tool offset for each individual tool that is probed to it and is stored in each tool individual page. I thnk like normal? T-1 L value offset, T-2 L value offset, etc. Is that what you mean?

I am anxious to try this setup again with everything I have gleened thus far.

Thanks
 
I can say for sure that the probe can and does enter the G54 offset if I use a probing program that I wrote for this specifically for the material top Z 0. Alternatively, I use
very short probing program for the touch off of the top of the hard block which does not set any offset at all. I think the best next step is to do what has been suggested with MDI G54 Z1 and see if a tool that has already been set to height of the block/tool setter is in fact 1" above the work piece. I didn't think to do this and spent way too much time trying to digest the numbers which make no sense to me.
I'm curious how and when do you activate the tool offset? (Like using G43 for instance) Typing into MDI and sending the tool to 1" above the part without an active offset will get you either nowhere or in trouble. It's confusing how manual or how automated your system is.
3.) Your tool length offsets should be positive numbers; they should reflect the actual, physical gauge length of each tool.
I disagree. The way he's doing it will be just fine. Either way, he's establishing a relationship between the Master Tool (Probe) and his cutting tools. That's all that really matters. Even if he has to move the knee 15" down to get the workpiece under the spindle, he'll still have the relationship established earlier.

BTW - where is Machine Z Zero on this machine? Does it reference the Quill at full retract only? Knee ineffective? That would be my guess.
 
I'm curious how and when do you activate the tool offset? (Like using G43 for instance) Typing into MDI and sending the tool to 1" above the part without an active offset will get you either nowhere or in trouble. It's confusing how manual or how automated your system is.

I disagree. The way he's doing it will be just fine. Either way, he's establishing a relationship between the Master Tool (Probe) and his cutting tools. That's all that really matters. Even if he has to move the knee 15" down to get the workpiece under the spindle, he'll still have the relationship established earlier.

BTW - where is Machine Z Zero on this machine? Does it reference the Quill at full retract only? Knee ineffective? That would be my guess.
for each tool, I activate the tool offset once the tool setter is triggered by (again Fagor) hitting the key F!, then Z, then enter at which point the dimension shows up in the L (length) box, then escape to activate the tool.

As for machine Z Zero, correct, Z fully retracted/home. The knee is powered, but not conected to the CNC functionality as of now.
 
#1) I understand and agree with the first two sentences. The 3rd sentence had me a bit confused, but as I read it the second time, I think it too makes sense since the delta in height is compensated by the G54 (or other) offset, is that right?

Yes, that is correct.
#2) does make sense now that I see it in words and digested it. Why would it change, it is a physical distance that is constant unless the tip brakes, etc

Exactly. All other tooling assemblies are the same as well; as long as the length doesn't physically change, there is no point in recording a change on the tool offset page.


Work and tool offsets can be established so that they have order and represent real dimensions. When this approach is used, it becomes easier to create a system that you can use to set up any job, with any number of offsets. You can even run multiple jobs on the table at the same time and keep things orderly without any room for error.

The method I am laying out is how most places set up machining centers for production runs. Some places even use remote tool setters; a guy in a tool room puts the cutter in a holder for you; he then puts it in a machine to check the gauge length, slaps a sticker on it with the tool's info and gives it to the operator. The operator types in the gauge length from the sticker and never has to touch off the tool - although you should still double check and size in appropriately.

#3) Having a hard time with this statement, or maybe don't understand it. If the material probe (tool #1) is 3" long and and the first tool (tool #2) is a 1/4" end mill with an OAL of 2" and part of it is in the holder, I get it being a positive number, but what about T-4, a 1/2 drill that is 5" long? Wouldnt that be a negative number?

Good question. It works by setting your reference (Z work offset for the tool setter) at the gauge line of the spindle - to simplify the explanation, we'll say spindle face instead of gauge line. They are not the same thing but it will work fine since you touch off all tool's on the machine anyway.

To explain this part easier, forget about the probe and tool setter for a minute. Let's use the machine as a generic measuring instrument:
Bring the quill all the way down until the spindle face touches the table; now call that Z 0.0. Next, run the quill back up, install a tool and touch that off the table.

Here is the important part to focus on: The number displayed on your DRO will be the exact distance from the spindle face to the tip of the tool. It will also be a positive number since the Z0.0 point was picked up from the shortest possible distance...the spindle face.
There will never be a negative tool length because the spindle face is zero.

The above method should be how you calibrate your probe z length. To recap:

1.) Touch off spindle face on table and set Z0.0.
2.) Load probe, touch probe tip off table to record a preliminary length in T01, L1
3.) Run the probing routine to probe the table; the measured value shown will be the difference between your preliminary T01 L1 offset and the actual trigger point tool length of the probe.

Let's say you touch of the probe manually and get 3.125". You then run the routine and get a measured value of 0.006". Add the 0.006 to your T01L1 of 3.125 = 3.131".

4.)Now probe the table again... your measured value should be 0.000 and your probe is calibrated. Write down your T01L1 number along with the date so that you have it in case it accidentally gets erased.


#4) Understood

Your next sentence for me is one and the same. The block that I made I surface ground to within a couple of tenths of the trip point of the tool setter so probing with the material probe to the block is more or less identical to a tool touch off to the tool setter.

Excellent, that is a very helpful tool.



The offset location of the for the tool setter is the tool offset for each individual tool that is probed to it and is stored in each tool individual page. I thnk like normal? T-1 L value offset, T-2 L value offset, etc. Is that what you mean?
Yes but no. You want this to be independent and have it's own location data stored somewhere else. You can use one of your work offsets to do this now. Later on when you begin working with macros, you can assign a variable location for the x,y and z locations of your tool setter program. For this example we will use G59.

Now that we have a know length for the probe, I will describe how to deal with the tool setter and the fact that the knee height is always changing.

1.) Pick up the center of the tool setter plunger by sweeping it with an indicator and set X and Y in G59 - X and Y will never change unless you physically move the tool setter.

2.)To pick up Z; Load the probe and bring it down close to your ground block. Take that preliminary Z number, subtract T01L1 from it and input the result as your G59 Z0.0.
3.) Run the routine to probe the block, make sure that it calls G59 to run the program and outputs data to update the same.

You will need to do step 2&3 anytime you move the knee, but only if you need to set tools that you don't already have good length offsets for.

When you set your z work offset for the part you are making, do the exact same steps as above; obviously, touching off of the workpiece rather than the tool setter block.

Important points of this concept:

Work offsets are recorded as spindle face to workpiece zero.

All tool lengths get recorded as the distance from spindle face to tool tip.

This keeps your tool lengths and work offsets completely separate and gives you a quick and easy way to measure a new tool, regardless of where the knee is positioned.
 
Last edited:
I disagree. The way he's doing it will be just fine. Either way, he's establishing a relationship between the Master Tool (Probe) and his cutting tools. That's all that really matters. Even if he has to move the knee 15" down to get the workpiece under the spindle, he'll still have the relationship established earlier.

Sure, that works as well but the numbers are abstract. They are not intentionally tied to a master because he is resetting the probe length each time. Some are longer than the current probe length and some are shorter.

Using the spindle face as the master will prevent losing all of your stored tool data in the event of a probe crash - which does happen to everyone eventually.

Renishaw probe calibration instructions state that a master of a known gauge length should be used when calibrating a probe or tool setter. In lieu of buying an expensive master, especially for a knee mill, the spindle face works fine.
 
for each tool, I activate the tool offset once the tool setter is triggered by (again Fagor) hitting the key F!, then Z, then enter at which point the dimension shows up in the L (length) box, then escape to activate the tool.

As for machine Z Zero, correct, Z fully ret

Yes, that is correct.


Exactly. All other tooling assemblies are the same as well; as long as the length doesn't physically change, there is no point in recording a change on the tool offset page.


Work and tool offsets can be established so that they have order and represent real dimensions. When this approach is used, it becomes easier to create a system that you can use to set up any job, with any number of offsets. You can even run multiple jobs on the table at the same time and keep things orderly without any room for error.

The method I am laying out is how most places set up machining centers for production runs. Some places even use remote tool setters; a guy in a tool room puts the cutter in a holder for you; he then puts it in a machine to check the gauge length, slaps a sticker on it with the tool's info and gives it to the operator. The operator types in the gauge length from the sticker and never has to touch off the tool - although you should still double check and size in appropriately.



Good question. It works by setting your reference (Z work offset for the tool setter) at the gauge line of the spindle - to simplify the explanation, we'll say spindle face instead of gauge line. They are not the same thing but it will work fine since you touch off all tool's on the machine anyway.

To explain this part easier, forget about the probe and tool setter for a minute. Let's use the machine as a generic measuring instrument:
Bring the quill all the way down until the spindle face touches the table; now call that Z 0.0. Next, run the quill back up, install a tool and touch that off the table.

Here is the important part to focus on: The number displayed on your DRO will be the exact distance from the spindle face to the tip of the tool. It will also be a positive number since the Z0.0 point was picked up from the shortest possible distance...the spindle face.
There will never be a negative tool length because the spindle face is zero.

The above method should be how you calibrate your probe z length. To recap:

1.) Touch off spindle face on table and set Z0.0.
2.) Load probe, touch probe tip off table to record a preliminary length in T01, L1
3.) Run the probing routine to probe the table; the measured value shown will be the difference between your preliminary T01 L1 offset and the actual trigger point tool length of the probe.

Let's say you touch of the probe manually and get 3.125". You then run the routine and get a measured value of 0.006". Add the 0.006 to your T01L1 of 3.125 = 3.131".

4.)Now probe the table again... your measured value should be 0.000 and your probe is calibrated. Write down your T01L1 number along with the date so that you have it in case it accidentally gets erased.




Excellent, that is a very helpful tool.




Yes but no. You want this to be independent and have it's own location data stored somewhere else. You can use one of your work offsets to do this now. Later on when you begin working with macros, you can assign a variable location for the x,y and z locations of your tool setter program. For this example we will use G59.

Now that we have a know length for the probe, I will describe how to deal with the tool setter and the fact that the knee height is always changing.

1.) Pick up the center of the tool setter plunger by sweeping it with an indicator and set X and Y in G59 - X and Y will never change unless you physically move the tool setter.

2.)To pick up Z; Load the probe and bring it down close to your ground block. Take that preliminary Z number, subtract T01L1 from it and input the result as your G59 Z0.0.
3.) Run the routine to probe the block, make sure that it calls G59 to run the program and outputs data to update the same.

You will need to do step 2&3 anytime you move the knee, but only if you need to set tools that you don't already have good length offsets for.

When you set your z work offset for the part you are making, do the exact same steps as above; obviously, touching off of the workpiece rather than the tool setter block.

Important points of this concept:

Work offsets are recorded as spindle face to workpiece zero.

All tool lengths get recorded as the distance from spindle face to tool tip.

This keeps your tool lengths and work offsets completely separate and gives you a quick and easy way to measure a new tool, regardless of where the knee is positioned.

This is a great write up and I understand it. I am going to print it out and keep it by the machine as a cheat sheet until it is second nature.

Thank you very much for the help. I will do this and report back as soon as possible.
 
This is a great write up and I understand it. I am going to print it out and keep it by the machine as a cheat sheet until it is second nature.

Thank you very much for the help. I will do this and report back as soon as possible.
I do have a somewhat unrelated question related to the tool numbering and CAM software. If I call the material probe T-1 in the CNC when I set up its length as you have laid out for me, and use Fusion 360 (in my case) as the CAD/CAM software, do I need to start the tool numbering for a given part from with T-2 so the CNC call T-2 as the first tool in the line up?
 
I do have a somewhat unrelated question related to the tool numbering and CAM software. If I call the material probe T-1 in the CNC when I set up its length as you have laid out for me, and use Fusion 360 (in my case) as the CAD/CAM software, do I need to start the tool numbering for a given part from with T-2 so the CNC call T-2 as the first tool in the line up?

I am not sure that I entirely understand the question. I use mastercam and it has tool numbers assigned to each tool in the library. You can change the tool numbers each time a tool path is created. It has hundreds of tools stored so I often have to manually override the tool number designated by the software.

My programs almost never end up with consecutive tool numbers. A program may start with T11 as a 2" face mill, then T23 a spot drill, T04 #7 drill, T8 1/4" end mill, and so on.

There may be a way that you can omit the T01 position in fusion, that way it will not post tool #1 if you'd like. Someone who knows fusion may be able to give a better answer.
 
I am not sure that I entirely understand the question. I use mastercam and it has tool numbers assigned to each tool in the library. You can change the tool numbers each time a tool path is created. It has hundreds of tools stored so I often have to manually override the tool number designated by the software.

My programs almost never end up with consecutive tool numbers. A program may start with T11 as a 2" face mill, then T23 a spot drill, T04 #7 drill, T8 1/4" end mill, and so on.

There may be a way that you can omit the T01 position in fusion, that way it will not post tool #1 if you'd like. Someone who knows fusion may be able to give a better answer.
I think you did answer my question. Yes, I can change the numbering in Fusion as you stated you do with Mastercam. Same scenario with the tool library and tools with numbers all over the place.

I was suspecting that prior to post processing, I edit the tool numbering such that it can be T1,T2 and so on or, since the CNC is using the assignment of T1 for the material/part probe, I can order the tools for the part in Fusion as T2,T3,T4 and so on every time I post a program if I choose.

Alternatively, I suppose I can set the probe to tool #50 or something since there is a slim chance that a program would have 49 tools.

Thanks again.
 
The OP has gotten some direction and seems to be on his way. All good there. Just some thoughts about earlier comments before bailing out.
Sure, that works as well but the numbers are abstract.
How so? The only thing any Machine Tool knows all on it's own is where home is. Without an active Work Offset set somewhere SW of home, no Positive numbers exist. It's only when machining takes place with respect to a Work Offset, do Positive numbers have any meaning at all. So remembering and/or setting a negative position from Home doesn't seem abstract at all.
They are not intentionally tied to a master because he is resetting the probe length each time. Some are longer than the current probe length and some are shorter.
No he is resetting a Work Height Offset. His Probe length stays the same just like all the other tools. The work heights he sets in his G54Z will always be the difference (plus or minus) from the Probe tool length, and by extension, the Tool Setter and the tools measured against it. I think the biggest problem the OP will have is always having the knee at the same place when measuring a new tool. This potential hick-up might be the best and only reason to consider Positive Offsets.
Using the spindle face as the master will prevent losing all of your stored tool data in the event of a probe crash - which does happen to everyone eventually.
If he crashes the probe, he simply resets the Probes tool length and continues on as before. It's the Tool Setter being crashed that might mess up the tool cart.

The benefits of Positive Tool Offsets in a shop with an offline Tool Setter feeding multiple machines is easy to imagine. No problems there. (Or here really) Still, I've never once in 20 years running multiple machines set a Positive Tool Offset. I have a feeling that the OP is not going to be able to maintain a large bank of set up and measured tools. That is unless he wants to invest a fortune in Tool Holders. So whatever route he takes he'll likely get good at over time do to repetition. I think he should use whatever setting type, pos or neg, that clicks in his head. The Positive Offset scenario has been carefully laid out for him and he seems to like it, so there is much good to be said for that. I tend to like the Negative version and suggest to the OP that if he gets going in the Positive direction and finds it iffy, trying his original Negative slant should not be out of the question. As we all know, both will work when applied correctly. Not knowing the Fagor system and seeing what the OP is seeing, makes it difficult to comment with complete certainty.

As far as Tool numbering and CAM. You are in charge of making up and applying your own Tool system. Meaning you can force the issue in CAM to suit your real world conditions. And just because a Tool was once called T2, there is nothing in the universe that says next time it can't be called T6 or whatever number fits at that time. You might try getting Tool Tags. With these, you can store the Tool Offset Height (or Gage Length) and carry it with the tool, making changing it's number as simple as entering in it's height (or length) setting into the control in the appropriate place.
 
The OP has gotten some direction and seems to be on his way. All good there. Just some thoughts about earlier comments before bailing out.

How so? The only thing any Machine Tool knows all on it's own is where home is. Without an active Work Offset set somewhere SW of home, no Positive numbers exist. It's only when machining takes place with respect to a Work Offset, do Positive numbers have any meaning at all. So remembering and/or setting a negative position from Home doesn't seem abstract at all.

No he is resetting a Work Height Offset. His Probe length stays the same just like all the other tools. The work heights he sets in his G54Z will always be the difference (plus or minus) from the Probe tool length, and by extension, the Tool Setter and the tools measured against it. I think the biggest problem the OP will have is always having the knee at the same place when measuring a new tool. This potential hick-up might be the best and only reason to consider Positive Offsets.

If he crashes the probe, he simply resets the Probes tool length and continues on as before. It's the Tool Setter being crashed that might mess up the tool cart.

The benefits of Positive Tool Offsets in a shop with an offline Tool Setter feeding multiple machines is easy to imagine. No problems there. (Or here really) Still, I've never once in 20 years running multiple machines set a Positive Tool Offset. I have a feeling that the OP is not going to be able to maintain a large bank of set up and measured tools. That is unless he wants to invest a fortune in Tool Holders. So whatever route he takes he'll likely get good at over time do to repetition. I think he should use whatever setting type, pos or neg, that clicks in his head. The Positive Offset scenario has been carefully laid out for him and he seems to like it, so there is much good to be said for that. I tend to like the Negative version and suggest to the OP that if he gets going in the Positive direction and finds it iffy, trying his original Negative slant should not be out of the question. As we all know, both will work when applied correctly. Not knowing the Fagor system and seeing what the OP is seeing, makes it difficult to comment with complete certainty.

As far as Tool numbering and CAM. You are in charge of making up and applying your own Tool system. Meaning you can force the issue in CAM to suit your real world conditions. And just because a Tool was once called T2, there is nothing in the universe that says next time it can't be called T6 or whatever number fits at that time. You might try getting Tool Tags. With these, you can store the Tool Offset Height (or Gage Length) and carry it with the tool, making changing it's number as simple as entering in it's height (or length) setting into the control in the appropriate place.
I really like this conversely presented information. It establishes for me that not only is there more than one way to accomplish a successful set up, but also make me think through, and understand all of this with a bit more clarity.

I have attached a few photos so you can see what I have in the works. Not sure if I had mentioned, but I am a home shop machinist with a passion for metal working. My shop is outfitted with mostly manual machines other than my CNC plasma with router adaptation that I built some years ago.This Southbend CNC replaced my old BP 9x 42 mill and I chose it over an affordable (subjective I know) machining center for its 12 x 58 table size. Maybe not the best decision, but I was less intimidated due to overall familiarity. I will press on and keep all of you helpful folks informed.

Steve
 

Attachments

  • Tool Cart.jpg
    Tool Cart.jpg
    791.4 KB · Views: 6
  • South Bend Mill Front 2.jpg
    South Bend Mill Front 2.jpg
    2.2 MB · Views: 6
  • South Bend Mill Side.jpg
    South Bend Mill Side.jpg
    403.9 KB · Views: 6
How so? The only thing any Machine Tool knows all on it's own is where home is. Without an active Work Offset set somewhere SW of home, no Positive numbers exist. It's only when machining takes place with respect to a Work Offset, do Positive numbers have any meaning at all. So remembering and/or setting a negative position from Home doesn't seem abstract at all.

No, tool length offsets and work offsets (can be) totally independent, without respect to each other at all.

Lets set aside the positive/ negative thing for a minute. My tool length offsets represent the actual, physical dimension of the tool from it's cutting tip, to the spindle face.

Yours represent the difference between the tool being measured and a master tool. By definition, a master can never change; it needs to be the exact same physical size always and forever - therefore, a touch probe cannot be a master.

It sounds like the simple difference here is that I am subtracting my current probe length from the equation in order to reference the spindle face. You are leaving the probe length and referencing your tools from the end of the probe.

I know the method you are using works fine. I'm not implying that you are wrong or that you don't know what you're talking about, I just do not believe that particular method is the best practice to teach.

Now, if you had an actual master that was shared across all of your machines, that would be different. Like one of these:


Either way, the whole purpose of that tool is to get an accurate measurement of the actual probe length from gauge line to probe tip. However, they can also be used as the master for setting other tools.

1.) Load the master
2.) Touch it off the tool setter.
3.) Subtract it's 4" gauge length and call that Z0.0 for the tool setter.

Now, every tool that you measure on the tool setter will be referenced from the gauge line and shown as a positive number. The instructions provided with a tool setter or touch probe will show that this is the proper way to calibrate it.

I think the movable knee is what throws in the extra confusion. On a vmc or bed mill, the tool setter is pretty much 'set it and forget it'; on the knee mill, the z position of the tool setter will need to be picked up each time the knee is moved. This is not a big deal but it does require that the operator stick to the traditional method of picking up tool lengths and calibrating the touch probe as well as the tool setter.

No he is resetting a Work Height Offset. His Probe length stays the same just like all the other tools. The work heights he sets in his G54Z will always be the difference (plus or minus) from the Probe tool length, and by extension, the Tool Setter and the tools measured against it. I think the biggest problem the OP will have is always having the knee at the same place when measuring a new tool. This potential hick-up might be the best and only reason to consider Positive Offsets.

No, the probe length is not staying the same. Here is the process that he is using for each set up, I copied it from the first post:

Here are my steps:

Home the machine.
Set the tool offset for the probe (tool #16) to 0.
Move the axes over a hard block that is the exact height of the tool setter.
Using a simple one line code, Z- until the probe is triggered.
Press F1 (Fagor Control), then Z, then Enter, then Esc to set the tool length for the probe.

Again sir, I do not mean to imply that my method is the only one, however I do believe that it is the best option given the situation.

I really like this conversely presented information. It establishes for me that not only is there more than one way to accomplish a successful set up, but also make me think through, and understand all of this with a bit more clarity.

I have attached a few photos so you can see what I have in the works. Not sure if I had mentioned, but I am a home shop machinist with a passion for metal working. My shop is outfitted with mostly manual machines other than my CNC plasma with router adaptation that I built some years ago.This Southbend CNC replaced my old BP 9x 42 mill and I chose it over an affordable (subjective I know) machining center for its 12 x 58 table size. Maybe not the best decision, but I was less intimidated due to overall familiarity. I will press on and keep all of you helpful folks informed.

Steve

Steve, whew you could do open heart surgery in that place! You should start a "members shop" thread, I'd love to see more.

One more thing, make sure all of your probe routines call the probe's length offset before running the program. I know that's probably a given, I just have to say it.
 








 
Back
Top