trying to determine why you wouldn’t want to set “Z” to machine base? Once you set Z to machine base you really would never have to set it again between different jobs, correct? Just wondering if I am missing something. It would be a benefit if you were doing 3d but I also thought it would also work for other projects.
Correct and also maybe not correct.
True the base will always be the same. But the same thing will be true for the bottom set point as the top set point, the bit length. Cnc is deductive manufacturing not additive so i assume thats why its done more from stock top.
Early versions of Carbide Create were unable to preview V carve toolpaths when origin was set to the bottom.
The big consideration is that if one sets the origin to the top relative to the stock, then the possible results of having the origin set to top/bottom are okay/harmless — either the file runs correctly (also set to top of stock), or it cuts air (set to the bottom), but if the file is set to bottom of the stock the two possibilities are file runs correctly (also set to bottom of stock) or disastrous, trying to rapidly plunge through the stock so as to cut the baseplate which is supposed to be where the stock is (file is set to top of stock).
It’s perfectly acceptable to do, so long as one never makes a mistake in where the origin is set — that’s usually not the case when folks are starting out, hence the recommendation for top of stock until there’s a reason not to.
Please note that one can get the advantages of not cutting into the baseplate by:
- setting the origin at the surface
- jogging up by the thickness of the stock
- setting the origin at that point
1 Like
My personal preference is to use the top of the spoil board for my zero, plus the thickness of the double-sided tape I use (it is very consistent in thickness). I do this because I work almost exclusively with wood and wood isn’t very consistent in thickness. I then lie to Carbide Create about the thickness of the material so it thinks it’s a little thicker than the thickness of the wood to allow for some variation. Sometimes, the first pass cuts a shallow cut, once in a while it cuts air, but subsequent passes cut the depth I’ve specified. In this way, I avoid cutting into the double-sided tape (it’s a mess when the bit gets all gummed up). When using more traditional workholding, it also avoid cutting into the spoil board, extending its life.
For those who prefer to use the top of the stock, my suggestion is to measure the thickness of the stock at the point you are going to set your Z-zero and use that as the thickness of the material. Again, I’d like and tell the CAD/CAM software that the thickness is a little more so the first pass doesn’t try to cut too deep on the first pass where the stock is really thicker than what was measured.
1 Like
Here’s my take from experience.
Zero Z to spoilboard ( plus 0.010" if you use two layers of blue tape and CA glue ) if your cuts will be all the way through the stock or if you are going to flatten the top to a certain known depth less than the thickness of the stock.
Zero Z to top of stock if you are not concerned with the thickness, and you are not going to cut all the way through the stock. If the top of your stock is not consistent in thickness all the way across, you’ll have some variations in slot depths and width of vcarves of letters etc.
2 Likes
Here is my own two cents on the topic…
Like in my case I have been zeroing to the top of the material for so long and have all my projects set as such, even though I’d like to try the waste board zeroing I will not do so. Should I want to run a previous project I fear I’d forget how it was set and have a major mess-up on my hands and with the price of wood I’d be really POed at myself.
The way I am working works well, so I’ll remain with the process I use and be happy.
1 Like
If you have an accurate way of measuring stock thickness, and decent stock, set zero on the bottom. If you don’t have these, zero on top. If you’re carving intricate details, flatten your stock and zero on top. These methods have worked well for me.
I use bottom of stock about 90% of the time. As others have pointed out the stock thickness must be measured accurately with top or bottom. The reason I use the bottom is I do not scar up my spoilboard nearly as much as when using the top. If doing a vcarve I will use the top as long as none of the cuts go through.
The only negative about using bottom is in Jog Rapid positions you must jog the router/bit to a space where the material is NOT. If you do a Z+6MM over the stock the bit will ram into the stock. After you get used to that you are good using the bottom. When I switched from top to bottom I rammed the bit into the stock a few times. Doooooh!!!
3 Likes
I made a habit of naming my toolpath files with important info, like what bit to use, and recently, a reminder to measure how far out my end mill should be to go through the stock without hitting the collet. If you were to try a new setting, point it out in your file name so you remember when you run it.
2 Likes
As others have mentioned, use what fits you or your job.
Since I mix from top to bottom I use the notes section. It pops up when you open the file in CC if you have created notes.
4 Likes
I have to agree with this… I’m such a creature of habit that if I tried to change now, i would probably ruin something and end up being super POed about it. It’s where I’m at with using mm vs in … I started with inch because I use Imperial measurements for literally everything else. Now I really want to switch to metric but I’m too afraid to because I know I’ll miss something and it’ll go bad quickly.
1 Like
First dont be afraid to change. Change is essential. I have used imperial so long I dont want to change and everything in my shop is in inches. However the metric system is more precise and under the covers everything is converted to metric anyway. So expand your mind and try it. You can always put a metric ruler up on the table to remind you what a MM is. It wont take long to learn something new. You learned how to operate your CNC.
1 Like
It’s just another numerical unit.
1 Like
I actually started with metric; it is really simpler. Imperial is more complicated. I started with metric because my first CNC was a 3018 Genmitzu by SainSmart. I still have it but never use it anymore due to its size.
I use Imperial mostly now but spend time with my calculator to get it right.
(25.4 Metric is 1 inch Imperial)
Nice thing about Carbide Create you can switch from Metric to Imperial in the job setup screen.
To save on errors just be sure to verify what you are using prior to each job.
Both systems are good but metric is simpler because everyone is based on 100. Imperial can be confusing using thousands or 1/64" or 1/32" and having to convert to tenths of an an inch. So metric is more straightforward in a woodshop. When I went to school I never heard of metric. So I learned imperial and have always used imperial. I could learn metric but at this point I am not interested in relearning. Kids today know about metric and can adapt to it. Old dogs can learn new tricks but not if they don’t want to. I am definitely an old dog and enjoy sitting on the porch. I don’t discourage any one learning new things.
1 Like
I don’t have that option from Fusion, but I’ve reduced my silly mistake rate by naming the files consistently.
Setup Name - 01 - Tool Name - FLSBZ.nc
Where the letters denote the zero position
Front Left SpoilBoard Zero
With appropriate substitutions for
Front / Back
Left / Right
Top / SpoilBoard
I still make inattentive human errors occasionally, but this helps.
5 Likes
I always zero to the top of my stock. Even If I am cutting all the way through I will always zero to the top of my stock. After that I will jog my bit over the spoil board and move the z axis down to the bottom of my stock right at the surface of the spoil board. The z axis readout on Carbide Motion will tell you the exact thickness of your material. I then use this measurement as my material thickness in Carbide Create. I have never cut into my spoil board using this method.
1 Like
Actually, due to the implementation on GRBL boards, metric really is more precise. The numeric values that can be represented internally to GRBL do have a limited precision, so if your units are inches, then the smallest possible increment in values represents a larger distance than the same increment in mm.
So, using metric allows you to specify distances that are 1/25.4 as large as the imperial ones.
The converse is also true of course, but the fact that imperial can specify distances that are 25.4 times larger than metric rarely comes in useful - you would have to have a very large machine to exceed the largest possible distance in metric.
3 Likes
So, bottom line, it’s the limitation of the machine, human error, and not the system.
However, both metric in 3 decimal places or inch in 4 decimal places are more accurate numbers than the steps/mm on these machines will resolve.
While 0.001mm (0.00004") is indeed smaller than 0.0001", the smallest move the machine can make is larger than both. (My HDM at 160steps/mm will move 0.00625mm or 0.00025" per step)
The only clincher then is the rounding error on circular interpolation end point check, which seems to occur far less often using mm. (I have not tested this using 5 decimal places in inch??)
6 Likes