X axis is off center

[Kenny Duval]

First question about the probe. Have you checked the runout of the probe. It needs to run fairly concentric to the centerline of the spindle.

[didu]

You can get a rough measurement with a cheap digital caliper it will be a nominal size

There is nothing on a 123 block that you could use as a gauge to measure anything with, the standard 123 block has a much bigger hole than .150 most holes are tap 3/8-16 so that would have around a .312 hole

Most standard probes are .200 this number has to be in you probing software for it to work correct or your offset will be incorrect

In the video I posted I quickly went over how I got the tip diameter, but basically, I put the probe in the center of a hole of a known size, then pathpilot runs a routine and sets the diameter. I think using the hole on a 123 block the way I did probably produced a little error but I don't think it's enough to produce the type of error I'm seeing. Also when I jog my machine to X0Y0 after probing it the tool seems to be centered pretty perfectly over the corner of the stock, so I think I'm setting the work origin well....

[didu]

First question about the probe. Have you checked the runout of the probe. It needs to run fairly concentric to the centerline of the spindle.

Yes! I checked it both with a dial indicator the way this person is and using the routine with pathpilot. I got it to have so little run out I can no longer effectively detect the runout with my dial indicator

[Kenny Duval]

Yes! I checked it both with a dial indicator the way this person is and using the routine with pathpilot. I got it to have so little run out I can no longer effectively detect the runout with my dial indicator

Then my next question is...

Is the rough size of the stock in the vise that size that you have told Fusion that it is? In the file you sent me the you have told Fusion the stock is 4.1 inches wide in X and 5.3 in Y. Is the rough stock actually that size? If it's not this could account for what you believe to be an error in the right side of the cut. If the actual stock is less than 4.1 inches wide and the math originates from the left corner then it will look like what you are seeing when the machine cuts with the information provided.

If you were to change your work origin to the center of the stock then even if the stock was undersized it would not look shifted you would just cut air for a bit before the cutter entered the material.

[didu]

Then my next question is...

Is the rough size of the stock in the vise that size that you have told Fusion that it is? In the file you sent me the you have told Fusion the stock is 4.1 inches wide in X and 5.3 in Y. Is the rough stock actually that size? If it's not this could account for what you believe to be an error in the right side of the cut. If the actual stock is less than 4.1 inches wide and the math originates from the left corner then it will look like what you are seeing when the machine cuts with the information provided.

I just rechecked the stock with my calipers, the width is 4.087(X) and the depth is 5.3055(Y), so I think my numbers are close enough? Also, quick clarifying question! Should I be setting my origin to the top center of the stock as was mentioned above, so that I don't have to worry about potentially having the size of the stock wrong? And if I did this what do I probe to set the origin off of?

[shred]

Keep eliminating variables and testing. I strongly suggest to stop using model box points for your stock unless you absolutely need to. As soon as you change the stock, Fusion can reset cut depths and all sorts of things.

Is the part its cutting the right size? Cut some smaller scrap or even bits of wood or plastic to get faster answers if need be.

If the part is positioned in the wrong place in the stock but the right size, most likely your offsets are wrong. If it's the wrong size then other things like the tools are set wrong.

You should be able to see everything simulate in Fusion to see what its going to do. Define your stock to match what you have, hit the simulate button and see if it cuts how you think it should.

Once it simulates correctly in Fusion, take that code back to the machine and see what happens. If you have an edgefinder or even a small drill to pick out 0,0 instead of the probe, try that to eliminate the probe as the source of problems.. (set Z by touching off the stock with some paper or whatever other method you like.)

[Kenny Duval]

I just rechecked the stock with my calipers, the width is 4.087(X) and the depth is 5.3055(Y), so I think my numbers are close enough? Also, quick clarifying question! Should I be setting my origin to the top center of the stock as was mentioned above, so that I don't have to worry about potentially having the size of the stock wrong? And if I did this what do I probe to set the origin off of?

No..working from a corner is fine as long what you do is consistent. Some times I work from a corner some times I go to the center it just depends on what I am doing. You should always tell Fusion that stock is a little larger than the actual size of the stock. This will make sure you ease into the cuts versus what would happen is you told Fusion the stock was smaller than the actual size of the stock. That's a recipe for a crash or snapping a tool.

So if we believe the probe is running concentric to the centerlne of the spindle, is calibrated well and we have both a good work coordinte system and an accurate measurement of the stock then we have to move to the next question.

Is the machine moving accurately in the X and Y axis. Have you checked and verified that when you tell the machine to move 1 inch in the control that it is accurately moving 1 inch?

[didu]

No..working from a corner is fine as long what you do is consistent. Some times I work from a corner some times I go to the center it just depends on what I am doing. You should always tell Fusion that stock is a little larger than the actual size of the stock. This will make sure you ease into the cuts versus what would happen is you told Fusion the stock was smaller than the actual size of the stock. That's a recipe for a crash or snapping a tool.

So if we believe the probe is running concentric to the centerlne of the spindle, is calibrated well and we have both a good work coordinte system and an accurate measurement of the stock then we have to move to the next question.

Is the machine moving accurately in the X and Y axis. Have you checked and verified that when you tell the machine to move 1 inch in the control that it is accurately moving 1 inch?

When you work from the center of a part how do you set the origin for it? Do you still just probe a corner? And when I enter my stock into Fusion, if I make the stock bigger (say rounding both sides up to the closest .25") will my part still end up being centered? I eventually need to flip these parts which is why I want to double check! I haven't verified that 1" is actually 1", but let me go check!

[didu]

Keep eliminating variables and testing. I strongly suggest to stop using model box points for your stock unless you absolutely need to. As soon as you change the stock, Fusion can reset cut depths and all sorts of things.

Is the part its cutting the right size? Cut some smaller scrap or even bits of wood or plastic to get faster answers if need be.

If the part is positioned in the wrong place in the stock but the right size, most likely your offsets are wrong. If it's the wrong size then other things like the tools are set wrong.

You should be able to see everything simulate in Fusion to see what its going to do. Define your stock to match what you have, hit the simulate button and see if it cuts how you think it should.

Once it simulates correctly in Fusion, take that code back to the machine and see what happens. If you have an edgefinder or even a small drill to pick out 0,0 instead of the probe, try that to eliminate the probe as the source of problems.. (set Z by touching off the stock with some paper or whatever other method you like.)

I haven't been able to get model box points to work so I've been sticking to using stock box points! I have a ton of aluminum scrap so I don't mind testing in it (I don't really want to clean my machine after getting wood in it lol). When you say that my offset is the issue if it's positioned incorrectly do you mean my work offsets are wrong or the size of my stock? (Does the size of my stock that I punch into fusion really matter, so long as it's set to something larger than my actual stock so it doesn't crash?). Watching the simulation in fusion everything looks perfect, which is why I thought it was an issue with the probe but it doesn't appear to be. I don't have an edge finder, but I'll try using a small drill to set 0,0 instead!

[Kenny Duval]

When you work from the center of a part how do you set the origin for it? Do you still just probe a corner? And when I enter my stock into Fusion, if I make the stock bigger (say rounding both sides up to the closest .25") will my part still end up being centered? I eventually need to flip these parts which is why I want to double check! I haven't verified that 1" is actually 1", but let me go check!

No you won't work from the same corner. You select it as your WCS and then probe to find the center of the material. Path Pilot has probing cycles for that.

If everything is calibrated correctly and working normally your part will indeed come out centered in the stock in X and Y.

It's very important that you are consistent in your setup. Again it is not right or wrong to work from any specific location. You just have to make sure that the location you pick to work from is what you do at the machine. The reason suggested to not use model points for your work offsets is that location usually isn't available until some material has been removed to exspose it. It's certainly never a good idea for a first operation. Using the corner or center of the stock is always the best option for a first OP. As I mentioned earlier I almost never work form the top of the stock either. It is usually either the front left bottom corner or the center bottom of the stock. Once you run that first OP and face the top of the stock then your original stock point has been machined away. Makes it hard to recover if something goes wrong.

[didu]

No you won't work from the same corner. You select it as your WCS and then probe to find the center of the material. Path Pilot has probing cycles for that.

If everything is calibrated correctly and working normally your part will indeed come out centered in the stock in X and Y.

It's very important that you are consistent in your setup. Again it is not right or wrong to work from any specific location. You just have to make sure that the location you pick to work from is what you do at the machine. The reason suggested to not use model points for your work offsets is that location usually isn't available until some material has been removed to exspose it. It's certainly never a good idea for a first operation. Using the corner or center of the stock is always the best option for a first OP. As I mentioned earlier I almost never work form the top of the stock either. It is usually either the front left bottom corner or the center bottom of the stock. Once you run that first OP and face the top of the stock then your original stock point has been machined away. Makes it hard to recover if something goes wrong.

I'm machining a feature right now that should be 1.5" by 1.5" so I can make sure the size of the part is correct. In the meantime, would you mind pointing me to a resource that outlines how to run the probing routines that will set the center of the part? If I try running a part with that origin and it still ends up not being centered I feel like that could help narrow things down. I also just like the sound of using that as my regular way of setting origins!

[Kenny Duval]

I'm machining a feature right now that should be 1.5" by 1.5" so I can make sure the size of the part is correct. In the meantime, would you mind pointing me to a resource that outlines how to run the probing routines that will set the center of the part? If I try running a part with that origin and it still ends up not being centered I feel like that could help narrow things down. I also just like the sound of using that as my regular way of setting origins!

Start at 6:25 in the time line. I don't particularly like their method of doing so but it does work.

[didu]

The feature I just machined came out to be exactly 1.500" x 1.500" so I think this has to be some type of issue with my stock size. I'll try remaking my initial part with this probing method and see if that fixes it because I'm out of ideas as to what else it could be!

[shred]

I haven't been able to get model box points to work so I've been sticking to using stock box points! I have a ton of aluminum scrap so I don't mind testing in it (I don't really want to clean my machine after getting wood in it lol). When you say that my offset is the issue if it's positioned incorrectly do you mean my work offsets are wrong or the size of my stock? (Does the size of my stock that I punch into fusion really matter, so long as it's set to something larger than my actual stock so it doesn't crash?). Watching the simulation in fusion everything looks perfect, which is why I thought it was an issue with the probe but it doesn't appear to be. I don't have an edge finder, but I'll try using a small drill to set 0,0 instead!

Don't lie to Fusion about your stock size until you know what it does when you do that. It can skip machining areas it thinks are beyond the stock, pick goofy starting points or it will by default try to center parts in the stock size you gave it (I much prefer to use 'offset from X, offset from Z' rather than 'center' for model position for these reasons)

Good news parts are coming out the right size, that eliminates a lot of possibilites.

I like to zero X,Y back left of the vise (assuming that's the fixed jaw). If you're running a lot of similar parts, Z off the bottom of the stock via parallels or jaw steps so you can find it again if needed.

Make one of your 1.5x1.5 parts, leave it in the vise and then re-probe it. If the corner is where it should be (offset from the stock by the amount you set or shown in 'center') then the probe is behaving properly.

[mactec54]

In the video I posted I quickly went over how I got the tip diameter, but basically, I put the probe in the center of a hole of a known size, then pathpilot runs a routine and sets the diameter. I think using the hole on a 123 block the way I did probably produced a little error but I don't think it's enough to produce the type of error I'm seeing. Also when I jog my machine to X0Y0 after probing it the tool seems to be centered pretty perfectly over the corner of the stock, so I think I'm setting the work origin well....

Are then that should be fine with the Probe setup or close but not perfect

Then all it can be is your work offset is incorrect in your drawings so your stock is larger then your part but in your software your X0Y0 most likely is your finished part

You will have to allow for the extra of the stock when you set it up or just change the X0Y0 in your drawing to the outside of the stock and reprocess the program

[mactec54]

Don't lie to Fusion about your stock size until you know what it does when you do that. It can skip machining areas it thinks are beyond the stock, pick goofy starting points or it will by default try to center parts in the stock size you gave it (I much prefer to use 'offset from X, offset from Z' rather than 'center' for model position for these reasons)

Good news parts are coming out the right size, that eliminates a lot of possibilites.

I like to zero X,Y back left of the vise (assuming that's the fixed jaw). If you're running a lot of similar parts, Z off the bottom of the stock via parallels or jaw steps so you can find it again if needed.

Make one of your 1.5x1.5 parts, leave it in the vise and then re-probe it. If the corner is where it should be (offset from the stock by the amount you set or shown in 'center') then the probe is behaving properly.

That is a bad practice you should not set the Z Axis offset to the bottom of the work, Z axis should always use a negative number to cut the part

[mountaindew]

That is a bad practice you should not set the Z Axis offset to the bottom of the work, Z axis should always use a negative number to cut the part

Now I am confused

[mactec54]

Now I am confused

If you have been / worked in the machine repair business Spindles Etc. ( you would not be confused ) you would know that more crashes happen when the user is setting there Z axis offset to the bottom of there part, damaged machine tables and Vices is a common sight in some machine shops, setting from the top of the part is more forgiving and have a lot less crash repairs from incorrect Z axes offset crashes

It's easy to look in the G-Code program and see exactly how far the Z axes is going to travel into the part, every Z axis negative number is easy to see

For Routers cutting wood, and having a sacrificial table, setting the Z axis offset to the bottom of the part can work very well

[mountaindew]

If you have been / worked in the machine repair business Spindles Etc. ( you would not be confused ) you would know that more crashes happen when the user is setting there Z axis offset to the bottom of there part, damaged machine tables and Vices is a common sight in some machine shops, setting from the top of the part is more forgiving and have a lot less crash repairs from incorrect Z axes offset crashes

It's easy to look in the G-Code program and see exactly how far the Z axes is going to travel into the part, every Z axis negative number is easy to see

For Routers cutting wood, and having a sacrificial table, setting the Z axis offset to the bottom of the part can work very well

I setup multi side parts where 1side of part 'top' z offset is set at top of the material. As you mention. All operations run.
Then the part is flipped over 2nd side 'bottom' z offset is then set to bottom of part or on parallels. The part is milled to exact z height based on model height from top to bottom. And any other features finished on that side. You end up with a part that has a accurate dimension based on 2 different z offsets.
To my knowledge this is only way I know of programing a consistent dimension using the z axis. Only other way is to deck off and measure and repeat until you hit that z dimension. That is a method for manual milling and very time consuming. Cnc i use the offsets to get the correct z dimension. I have never seen anyone that does it a different way in a CNC program.

At machine all I do is make one part and set offsets as I flip part for 1- up to 6 sides. Using stops to locate material.
When finished with first part, I can repeat the process using all the offsets set the first time and make as many complete parts as I want.
Simple, repeatable and accurate. All in one g code program.
i also dont create a g code file for each side, you would end up with 1 to 6 g code files for a single part model. Over time you end up with thousands of g code files to manage. People do it that way but i never have. My cam makes all this easy to setup, compile and simulate a complete part before i ever go to machine with just one file to make the part.

[mactec54]

I setup multi side parts where 1side of part 'top' z offset is set at top of the material. As you mention. All operations run.
Then the part is flipped over 2nd side 'bottom' z offset is then set to bottom of part or on parallels. The part is milled to exact z height based on model height from top to bottom. And any other features finished on that side. You end up with a part that has a accurate dimension based on 2 different z offsets.
To my knowledge this is only way I know of programing a consistent dimension using the z axis. Only other way is to deck off and measure and repeat until you hit that z dimension. That is a method for manual milling and very time consuming. Cnc i use the offsets to get the correct z dimension. I have never seen anyone that does it a different way in a CNC program.

At machine all I do is make one part and set offsets as I flip part for 1- up to 6 sides. Using stops to locate material.
When finished with first part, I can repeat the process using all the offsets set the first time and make as many complete parts as I want.
Simple, repeatable and accurate. All in one g code program.
i also dont create a g code file for each side, you would end up with 1 to 6 g code files for a single part model. Over time you end up with thousands of g code files to manage. People do it that way but i never have. My cam makes all this easy to setup, compile and simulate a complete part before i ever go to machine with just one file to make the part.

Your cam is no different than what any good shop would have

What ever suits you can do but in a real machine shop this would not fly, when you setup your first operation you usually machine all 5 faces , the second operation can be added to the same program or be a separate program which is more efficient than what you are doing