Material setup with different Z-zero's

[Dan m]

Is there a way to have one .cnc file that has tool paths with different z-zero's?

What I'm trying to do is have one file that for example has a tool path that has a z-0 to the top of material for machining that doesn't cut all the way through, then in the same file a different tool path z-0 to the machine bed for through cuts. I've tried to do it but it recalculates all the tool paths to one or the other, not both within the same file.

Right now what I have to do is have one file with the z-0 top of material then program a separate file with the z-0 to the machine bed. It's a pain and adds time to the CAM programing as well as the machining.

I know I can do it all from top or bottom, but it's not nearly as accurate as using my tool setter coupled with my m6 macro. Right now when I touch off my tool setter off the machine bed and do a through cut the cutter doesn't touch my spoil board and doesn't leave any material behind. I like the fact that my spoil board is still perfect. Doing it this way I don't need to add more ops with the band saw and belt sander like a lot of guys Ive seen doing when they z-0 to the material and it doesn't cut all the way through due to material inconsistency's. I also don't have to worry about cutting into my spoil board surface, I like it flat and with no lumps. To me adding additional work to cut out your parts kind of defeats the point of a CNC.

So if there is a way to have different z-0's in the same file please let me know, I'm surprised that from my searching of the forum that this hasn't come up before from what I can tell. If it has been addressed please let me know where the thread is and how to do it. I'm very new to Vectric, and wouldn't be surprised if it does allow this and I just haven't figured it out yet.

Thank you,
Dan

[IslaWW]

You are trying to generate 2 files that do the job of one. If you have a Z setter that sets the bit that well, measure the material and cut it all with the Z ref to the Spoilboard. There is no logic to back up what you are trying to do. Pick a lane! In the long run a toolsetter that is Z ref to Spoilboard will be much more consistent and repeatable than setting Z ref to material top, as material surface is seldom as flat as a Spoilboard is surfaced.

[4DThinker]

When it is critical that I don't cut into my spoilboard, but I want Z0 to be on the top of a board I do home the bit on the spoilboard, but instead of accepting the default (Z=0) at that position I enter my board thickness with a negative in front of it. When my board is .75" thick, for example, I enter -.75 for Z. This is after setting up VCarve with Z=0 on TOP of the material.

I'm not sure if that is exactly what/why you want to use two Z values, but it results in an unmarred bed with all through cuts completely through.

4D

[Dan m]

You are trying to generate 2 files that do the job of one. If you have a Z setter that sets the bit that well, measure the material and cut it all with the Z ref to the Spoilboard. There is no logic to back up what you are trying to do. Pick a lane! In the long run a toolsetter that is Z ref to Spoilboard will be much more consistent and repeatable than setting Z ref to material top, as material surface is seldom as flat as a Spoilboard is surfaced.

I'm not trying to I have been doing it this way lately.

One file does the detail machining where starting from the top is important ie pocketing, engraving, 3d contouring ect... and one file does the through cuts. I didn't feel like going out in the shop and measuring all the different pieces of wood marking them and setting up a different cut file for each piece if the wood thickness varied "it usually does in my experience".

The only way to make a part repeatable would be to either touch off the top of the material, surface the material so the thickness is consistent on all the different pieces, or have a separate cut file for each piece of wood that has a different material thickness.

The reason I wanted to do it in one file is so I don't need to worry about measuring the material thickness from one piece to the next and have multiple files for the same part. So doing it the way I am currently, I will have two files that sit in the project file on the CNCPC that never need to be edited. Not the potential for having to out put a new file every time I get a piece of wood that has a different thickness than the last. No matter what I'm looking at needing multiple cut files for the same part unless it's only being run one time and never again or its a part that only requires a through cut or a part that only requires surface machining.

Do you understand why I want to pick both lanes now?

Dan

[IslaWW]

No

[Dan m]

No

So you don't understand why I don't want to edit my cut file every time I run the same part on a new piece of material? If wood had the same tolerance as a piece of aluminum plate then I wouldn't worry about it, but it doesn't. Example right now I have two boards both Popular, one is .80" thick the other is .77" I have a engraving tool path that has a cut depth of .03". Now do you understand what I'm talking about? In order to get the same doc I would either need to touch off the top of each board or have two cut files. I'm sure now you understand what I'm talking about and why I would want to z-0 to the top for engraving and z-0 to the machine bed to cut the part out. Or I can do it your way and on one of the pieces either air cut the engraving or go 2x the desired doc depending on what board went on first and what thickness I entered for the material.

What am I missing? If I'm wrong on any of this please let me know since I'm new to v-carve. I'm trying to understand how the file wouldn't need to be edited every time the material thickness varied.

Dan

[gkas]

So, add a first toolpath that will mill your wood to your preferred thickness. If you pick 0.75, then everything gets milled down to that dimension. You can even have your toolpath ignore areas of screws/clamps.

Flatten.crv

Plane board and exclude clamps

(47.5 KiB) Downloaded 41 times

[Dan m]

So, add a first toolpath that will mill your wood to your preferred thickness. If you pick 0.75, then everything gets milled down to that dimension. You can even have your toolpath ignore areas of screws/clamps.

Flatten.crv

That's definitely a option, will add another tool change and more time. I have done this before with some wood that wasn't flat, and is honestly the right way of doing it if you don't mind the extra time and work. I still would like to see the option for different tool paths, but maybe its more complex to add to the software than it looks. But if I'm the only one that would find the option useful in all the years Vectric has been around its not going to happen. I'll have to think of how I want to do it going forward, doing two different files doesn't take that much more time. If I get a ATC than adding a surfacing tool path will work well too.

Thanks for the input,
Dan

[IslaWW]

No

So you don't understand why I don't want to edit my cut file every time I run the same part on a new piece of material? If wood had the same tolerance as a piece of aluminum plate then I wouldn't worry about it, but it doesn't. Example right now I have two boards both Popular, one is .80" thick the other is .77" I have a engraving tool path that has a cut depth of .03". Now do you understand what I'm talking about? In order to get the same doc I would either need to touch off the top of each board or have two cut files. I'm sure now you understand what I'm talking about and why I would want to z-0 to the top for engraving and z-0 to the machine bed to cut the part out. Or I can do it your way and on one of the pieces either air cut the engraving or go 2x the desired doc depending on what board went on first and what thickness I entered for the material.

What am I missing? If I'm wrong on any of this please let me know since I'm new to v-carve. I'm trying to understand how the file wouldn't need to be edited every time the material thickness varied.

Dan

I understand completely what you are trying to do. Cut shallow depth engraving on a varying surface height and then make sure that you do not cut into the Spoilboard. But that was not your question, which was "Do you understand why I want to pick both lanes now?" I understand your problem, I do not understand why you chose multiple zero locations to solve it.

Having done a few production runs of 100+ plaques with customer supplied materials which varied in thickness like yours and no money in the job to surface them, I used a common process that Thermwood calls "ZSHIFT". This variable addition uses a standard, generic thickness for the file. Right before the file run, actual thickness is entered as a variable, the math is done and the table zero position is shifted up or down to match that thickness for all but the last pass, which is run at the original table zero.

[Dan m]

No

So you don't understand why I don't want to edit my cut file every time I run the same part on a new piece of material? If wood had the same tolerance as a piece of aluminum plate then I wouldn't worry about it, but it doesn't. Example right now I have two boards both Popular, one is .80" thick the other is .77" I have a engraving tool path that has a cut depth of .03". Now do you understand what I'm talking about? In order to get the same doc I would either need to touch off the top of each board or have two cut files. I'm sure now you understand what I'm talking about and why I would want to z-0 to the top for engraving and z-0 to the machine bed to cut the part out. Or I can do it your way and on one of the pieces either air cut the engraving or go 2x the desired doc depending on what board went on first and what thickness I entered for the material.

What am I missing? If I'm wrong on any of this please let me know since I'm new to v-carve. I'm trying to understand how the file wouldn't need to be edited every time the material thickness varied.

Dan

I understand completely what you are trying to do. Cut shallow depth engraving on a varying surface height and then make sure that you do not cut into the Spoilboard. But that was not your question, which was "Do you understand why I want to pick both lanes now?" I understand your problem, I do not understand why you chose multiple zero locations to solve it.

Having done a few production runs of 100+ plaques with customer supplied materials which varied in thickness like yours and no money in the job to surface them, I used a common process that Thermwood calls "ZSHIFT". This variable addition uses a standard, generic thickness for the file. Right before the file run, actual thickness is entered as a variable, the math is done and the table zero position is shifted up or down to match that thickness for all but the last pass, which is run at the original table zero.

So how do I use zshift with vectric? Where does the variable get added? In the PP? Where is the thickness entered the controller? It sounds like something that is beyond my current skill level.

Oops, I just realized what you're talking about with the variable in V-carve.

My problem with doing it that way is I don't use my CNCPC to design anything it doesn't have any programs running other than what windows comes with and Cnc12 it's not even connected to the internet. My design computer is in the office and never goes in the shop. So all my cnc jobs get downloaded via flash drive and go into job folders. Once a design is production ready I don't look at it again other than loading it to cut. I also don't change my tools for each job, all my tools are set up for specific types of materials and once I get the optimal feed and speed for the tool in the specific material they aren't touched again in vectric. It was a lot of set up but now it makes programming tool paths super fast. Example 0.25" end mill is set up multiple times with different tool numbers with different feed and speed for different types of material and so on for my other tools. Probably not how you would do it but it works for me.

The way I'm doing it works for me and helps eliminate human error, the machine does all the work and since the cut through tool path is a separate cut file there is no way to z-0 in the wrong place unless I don't read the notes or the file name. IDK it's very possible after a few months of running the machine I'll change my mind on wanting the ability to have two z heights. I'm still working on the most efficient way to run jobs with the the lowest chance of having a brain fart and ruining material or breaking tools.

Here's a picture of a part that I zero to the top and bottom.

Dan

[dealguy11]

If this was in my shop I would just run all the wood through a planer or wide belt sander to make the material a standard thickness beforehand. That eliminates all chance of thickness error (unless you set up the machine wrong!).

Also I do all this work from the spoilboard. Used to switch back and forth. After a few catastrophic brain farts I decided to take Gary's advice and "pick a lane". Almost setting your machine on fire by driving a bit into it by accident does focus you somewhat.

[Rcnewcomb]

Almost setting your machine on fire by driving a bit into it by accident does focus you somewhat.

Amen.

[Leo]

Agreed - pick a lane

For me, it is top of material. I have my reasons, so does everyone else.

Just changing tools and keeping track of what is going on.

I don't want to add another variable.

Been doing this for more that 10 years at home and 3 times that in industry.

Never had a reason to have multiple Z zero points

[Dan m]

The tool change macro I use prompts me to do one of 3 things
1) skips setting z height uses what the last setting was
2) set tool height with touch plate and move to tool offset device record offset
3) goes to fixed tool offset device and records new z-zero

I can call out notes during the tool change within the macro so there's no way to mess it up unless I don't read the call out.

The way I'm currently doing it eliminates having to worry about inconsistency's in the material. The worst thing that could happen is on the cut through tool path it could potentially air cut the first pass which would suck and waist time or take a deeper first pass but since my doc's are pretty conservative I'm not worried about breaking cutters. I'm just trying to not waist time doing unnecessary cam work every time I rerun a part I've previously cut if I can avoid it. I understand some times its unavoidable if you're for example switching material types or the thickness varies more than a couple hundred tho.


And thanks Gary I looked up the Thermwood z-shift and that's a nice option but if I'm understanding the way it works correctly. It would have to be a option that Centroid added to CNC12, maybe you can add that to the list for the Router version seems very useful and much better than what I'm doing? Did you work for that router company, or just have one of their machines?


Thanks guys for the input and advice. Looks like I'm the only one that would find different z settings useful so I will just move on and after more time with the machine figure out what works best for my work.

Thanks again,
Dan

[mtylerfl]

Well, there is way to create a project using both Z zero Top and Z zero Bottom. You would still have two separate cut files, but just one Project file.

That is, setup a job as two-sided and select the option to Set Z zero from the same side.

Not particularly simple nor necessarily practical IMO, as you would need to pay very close attention to how you layout the project between the Top and Bottom of the material - especially since you would NOT be actually flipping the material over.

But, one side you would layout the “stuff” you want zero at the top surface and the other side you put the stuff you want your zero at the bottom surface (I.e., the spoilboard).

Easy to make a mistake doing a layout like this when not actually flipping the material over. So if you attempt - don’t blame me if things go horribly wrong!