Z zero

[George_Gerhard]

I was wondering how many people make Z zero the bottom of the part instead of the usual top, and if so how do you set up the retract and feed plane settings. Many of my customers want the bottom to be zero because they cut wood and the material thickness varies quite a bit, and face milling the thickness is not an option. Making zero the bottom guarantees the blind operations will be the same from the bottom. Currently I make top of stock equal to material thickness, feed plane is absolute, material thickness plus .1 and retract is mat. thickness plus .25

Depth is 0 if the cut is through, but if blind then it is material thickness minus depth or how much is left. Using incremental does not work when there are many parts to be cut, as in a nest.

I am thinking of setting all the parameters as if zero is the top then shifting the z in the post.

Anyone else have ideas?

many thanks

George

[Guest CNC Apps Guy 1]

I ALWAYS make Z0 the bottom of the material. I draw my stock and then add say .1 above that for retracts and so far I've not had any probllems.

 

I like it because the bottom NEVER varies.

[Zero]

I use the table as zero on most of my parts, unless its some kind of cavity or it's getting flipped and I've faced off the top.

 

quote:

---

I like it because the bottom NEVER varies

---

same here...

 

My Clearance and Feed Plane are always set on Absolute, at a safe distance above the part. Feed plane I always set on Incremental at about .25. Never fails this way

 

[ 09-21-2003, 02:34 PM: Message edited by: Zero ]

[Thad]

Z0 is dictated by the file/print. Except for very rare circumstances, Z0 is the mounting surface (or bottom) of the detail. Like James said, that never changes. If there is work on the top and bottom, Z0 stays the same and we use the WCS for machining.

 

As far as the parameters go, my defaults are set to absolute 2.0 for clearance, incremental retract .25, incremental feed plane .1, top of stock and depth are set to absolute 0 (for safety...well kind of ) Since we probaly do just as much work on the bottom of a detail as we do the top, it's hard to set the defaults because they're probably only accurate 60% of the time. Since doing this for over a year, I know what I've got to look for and what always gets changed, so I don't have any problems with it.

 

Thad

[Müřlıń®]

I always use the top of my die or a tooling block. I am not tied down to a certain thickness as the height is shimmed.

 

.25 clearance absolute

.25 rapid retract absolute

.25 feed plane inc.

top of stock 0

 

 

Since I dont use tooling offsets, I just zero my tools all in the same spot on a Jo Block. This way I don't have to worry about heat expansion causing me any problems going from tool to tool. I will zero off the tools as I need them.

 

If I was doin' wood that varied in size, I would use the shortest one to set zero. If the tallest one was more than 1/4" thicker, I would adjust the retract values and watch the first cut

 

 

Murlin teh unorthadox

[crazy^millman]

Well for me I do my frist side of the part using the top of the part. I then fip the part around the origin and then use Z0 on the bottom of the part. I would make sure if you are doing 5th axis or 4th axis machining you apporach it different. I make the center of rotation my Z0 and I make the top of the part my Z0 for wind and unwinds. I find that is you are doing a tall part say 22" tall and have the wind and unwinds at the standard 10" then it could possible be a boom bang crash. I have seen and done it many ways and also have had Z0 a critical surface I was controlling on a part.

 

I just do what feel comfotable to me and sure that I can get away with. I soemtimes have incremntal and absoulte mixed it is all what you feel you can do and feel comfortable getting away with. Be safe, be sure, check and double check for it is always easy t otake it off but alot harder to put in back on.

 

Crazy Millman

[George_Gerhard]

thank you for all the responses. Believe it or not, many of my customers complain about using absolute numbers, they seem to get confused with depth. If the material is .75 thick and the pocket is .5 deep from the top then depth is .25 above the zero point. They would like to just be able to input what the depth is.

I also like teaching them to make zero the bottom of the part, because after they make code, I have them check the code for Z- If there are any this is a potential crash.

I saw a program called artcam which has on the setup page, two radio buttoms one on the top of the part and one on the bottom, you just pick the one you want ( zero top or bottom) then you can just input a depth in incremental.

 

regards

George

[Trevor Bailey]

For all of the fixtures I made for carving necks, I made Z0 bottom. I put all retracts in MC incremental and added distance accordinly(SP). Height 1' increm, retract .75 and feed .100. Never had any issues since you either pick surfaces or other geometry to tell MC where you part is.

[Müřlıń®]

quote:

---

If the material is .75 thick and the pocket is .5 deep from the top then depth is .25 above the zero point. They would like to just be able to input what the depth is.

---

You can zero off on a .75 Jo Block. You will still be holding the correct distance from the table, and you will be able to set your depth of pocket to any number with out any calculations.

 

Your varing thickness won't matter because you will clear it on the retract height.

 

 

Murlin teh just throwin' ideas at yas

[Nominal]

I try to always set my origins at the same place I'm locating the part from. With a hunk of raw stock it would be the bottom side, down in a vise or clamped to the table. For castings you should be setting zeros at the datums. What ever you call your origin, the only thing that will be constant from part to part are the distances from whatever you're locating from.

[chris m]

Depends on what we're making But I like to set Z0 at the top of the part whenever possible. I like to be able to look at the code and see where the tools are without having to calculate anything; plus you know instantly that Z- always means inside the part. When milling from solid or castings I always chip the top surface with the very first op so I know where the part is after that, if working with a part that has the overall already finished, our parts are so tightly toleranced that the top surface can't be off more that about .010, regardless of the part size.

 

Retract .100 (sometimes .200 on long-chipping mat'l peck drilling)

Approach / Retract Clearance .250

 

C

[heeler]

We use the "theoretical" top of stock as 0. We then set the bottom of the stock to a known -Z value. That way like Chris, whenever you see a -Z you know that you are in the material envelope. It also makes it so that you don't have to set Z on every part, just face the material to the thickness that you want. I know that when I am running a machine, I know where the tool is going easier with this method. When I have ran programs that someone did with Z on the bottom, It really confuses me on where the drill is going to rapid to, before it starts the drill cycle.

 

JM2C

Glenn

[kathy]

For our panels, I set Z Zero to the TOP of the panel. One reason is that the insert holes are than -.___ absolute value down into the part, and that number corresponds to the spec!. Also, as the panel thickness may vary, we know right where we are when setting to the top. Turning the panel over, SETUP B is the TOP of the backside of the panel. If we have a tight flatness tolerance for panels on the Komo, we run a Renishaw probe over the hole pattern, and adjust the depths using that data.

 

For flat sheet metal parts, I set Z Zero to the top of the table (bottom of the stock). My co-heart in the office here likes to set to the top of the material. But on our Komo, it’s easy to take the tool offsets on the table right by the controller.

 

So Z Zero should be set appropriate to the part datum and the part setup!

 

This is what is nice about a flexible CAM system.

 

Kathy

[bryan314]

For us most steels get two setups. The first setup Z0 is set to the top. The steel is flipped and second setup Z0 is bottom of stock.

 

We always use absolute increments. We had a few too many surprises back in 7 and early 8 when trying incremental. Just a little gun shy.

 

Also of note we're under penalty of death if we move a detail out of die position. So we make heavy use of named planes. Just orientate and set Z0 as needed.

 

Of course, any of this can vary from steel to steel, job to job as necessity dictates.

 

Bryan

[CAM-mando]

+1 Chris and Heeler.

 

For us ...

 

"Top of part" means table Z + theoretical part height. So it doesnt vary but numbers are still from top which we usually prefer.

 

"Actual Top of Part (or stock)" Means pick up Z on the work piece itself.

 

CAM

[George_Gerhard]

Kathy

I noticed you have Komo. My company was the Komo dealer for the northeast for the last 9 years. I know these machines very well, both electrically, and mechanically. Should you ever have a question please dont hesitate to ask

regards

George

[Fig sign]

It depends !

 

I mostly use z0 at the top of the part but when I must catch bottom I use height from the bottom .

Also at my recent work place doing 4-axes jobs many times it was easiest to have Z0 center of the 4`th axis .

It can be anywhere just must be convinient for you and if you are working solo like me it`s not a problem.

When you have operators a good idea to make some standart approach .

 

Iskander s!z G0 Z-2 -crash ????

[chad fisher]

This might sound a little different but in our shop we teach all our mill operators to run this way.

1st touch all tools from a 6" block from machine table.

2nd calculate vice/parralle/part thickness and subtract value from 6".

3rd enter that # into fix offsets.

Most of our work is in 8" or 6" vices so 3.5 and 3.188 is a standard for all vices in our shop. We do most all programming for Z0. being top of part. Plus if operators switch machines they will know where the tlo's are if using some tools for differnet parts.

[MetalMarvels]

I always set my tools to 2 inches above my table and set my fixture height accordingly. I use 2.000-inches primarily because that is the height of my tool setter. The nice part about doing it this way is that I can change a tool at any time and be assured of correctly setting lool lengths. Depending on the part, I will use the top or the bottom as the Z0 point. Mostly, I use the bottom on raw stock since the thickness can vary somewhat. I also typically use the back left corner of the part as x0 y0, but will vary that as required by the part (for example the back left corner doesn't work real well with 4th axis parts).

 

I had long ago been taught to set my tools directly to the top of the stock or part, which works fine for a one-off part. However, you soon come to realize that a tool changeout in the middle of a part is a disaster because your reference height may have been milled away.....

 

[ 09-24-2003, 03:42 PM: Message edited by: MetalMarvels ]

[ScottyB]

On our Heian Z0 is the top of the part and in Inches.

 

On our Weeke Z0 is the bottom of the part and Metric.

 

I've been helping a friend with a Multicam and Z0 is the bottom and it's in inches. (I'm still trying to figure that machine out!)

 

I generate code in Absolute, but when I write macros by hand I like Incremental.

 

No, wait maybe the Heian is Metric...damn my brain is fried.

 

ScottyB. teh confused.

[BernieT]

I set Z 0 at top (parting line) with molds.

 

I set Z 0 at bottom of stock (top of table or top of parallels in vise) whenever the top of stock will be machined away.

 

I set Z 0 at middle of stock when machining a model that is symmetrical from top to bottom. Example: Tennis racquet.

 

Interesting to read this thread, amazing how many different ways to set-up a job. All make you think.