What is the G Code to pause CNC so we can exchange milling bit?

[cekuhnen]

Does anybody know what G Codes you need to use to

after an adaptive pass:

pause the CNC

Move it to somewhere else

Put in a different CNC milling bit

registers the CNC milling bit (possible different length)

continue CNC millin for the next task such as contour

[Steinwerks]

This is going to depend pretty heavily on your machine.

M00 is a program stop. If you need to physically/manually touch off the tool, you may want to consider simply posting your toolpaths separately (can be done from the same setup though) so that they can be run independently without worrying about changing tools in the middle.

If you have a way to probe the tool automatically after changing it manually it can be worked into the post processor, but you need to know how that happens at the machine.

[cekuhnen]

@Steinwerks

we try to figure out how to re register the start position after the first path because the foam block is cut and we do not have the center point on top of the foam block any more.

so how would you make sure that with a second G Code for contour it would work perfectly on the result of the first adaptive path?

This is the custom build CNC we bought:

the company is out of business so I do not even know the name we have the machine since 3 years and just got it somewhat workling

[LibertyMachine]

If you have not moved the part on the table or changed the work offset (G54-G59) any, the X and Y of the code will be good. The concern I would have is in the Z axis. How did you touch off the last tool, was it on top of the part/raw stock? Well, now that is gone...

If it was top of the part, do you have another piece of that same sized material that you could use somewhere else on the table to facilitate touching off a new tool?

[cekuhnen]

@LibertyMachine

Well that is actually our mystery right now. Different tools can have different sizes so we need to accommodate for that.

the Fusion interface gives you few start points but they are all well on the initial stock like in the screenshot below

I am not sure how one could or should use those points on the ground plane or inside the stock volume ?!

is there a way on the build platform next to it to find rest position like 2 cm away from the stock and then

after a tool chance use the build platform to find the correct z position?

we also have a z click plate but our CNC software crashes / freezes after we trigger the find z position.

[LibertyMachine]

---

@cekuhnen wrote:

@LibertyMachine

Well that is actually our mystery right now. Different tools can have different sizes so we need to accommodate for that.

the Fusion interface gives you few start points but they are all well on the initial stock like in the screenshot below

I am not sure how one could or should use those points on the ground plane or inside the stock volume ?!

is there a way on the build platform next to it to find rest position like 2 cm away from the stock and then

after a tool chance use the build platform to find the correct z position?

---

During the initial setup stages, you can establish any point you would like as your origin point. Top, bottom, left, right, anything basically. Thing is, you sort of need to keep that location.

Now, it is technically possible to switch origin points halfway through a job, but the likelihood of tools blending well to previous cutting operations are very slim, without a decent amount of trial and error.

The above statement concerns mostly the X and Y repeatability of switching origin points along the X and Y axis.

Now, what you "could" do is shift the Z origin down to the bottom plane. However, if you touched off on raw stock that was oversize from what you planned, you would be off that amount when you started to cut on your new tool.

Lastly, yes, you could use the "build platform" next to the part to establish tool heights. What I would do:

Take the tool that is still in the spindle (assuming the first tool is still in?) Bring it down to near that height, using a small block of a known height (gage block, bar stock, etc). Bring the tool down until the block barely fits under the tool (careful not to damage the tool). Now, compare the Z value to that of it's initial touchoff. The difference would be the Z shift value and it would become a positive value that is placed into G54 Z offset (WARNING: I'm assuming your control actually is working like a convention CNC control, your results may vary)

Now you should be able to touch off all your tools on that build platform

[cekuhnen]

@LibertyMachine

I am new to CNC so I will have to look into what you suggested but based on the concept you explain this makes sense

Our CNC router software allows us to edit the code instead of only using the software Fusion offers after making the G Code.

[LibertyMachine]

If you were to touch off your new tool at a lower point than the original tool, you would have to do one of a few things. First, you need to know that difference from the original height to the new height. This can be obtained if you have another block of foam from the same bar. The other method would be to locate the high point (using a test or dial indicator) of the machined surface, write down the Z value, travel over to the new touch off position and bring the indicator down (by moving the Z axis) to the new height. This new Z value, minus the previous Z value of the top of the part, is your Z difference. You will also need to keep in mind how far below the stock surface were you cutting to reach this high point. Were you running default of 1-2mm stock allowance on all sides, or were you using a known figure?

You can either input this into your G54 workoffset as a POSITIVE value, or you can shift your entire program also POSITIVE. I would not recommend the second option because it is more of a chance of having a crash. If you need to repost some code and you forget to shift it again......ooooops...