Coordinate System Choice

[jon_fallon]

Starting to use multiple tool holders for tapping and drilling, and am curious as to how everyone handles the tool length offset. An LED face setting tool is used that is 2.00 inch height.

1st Approach:
Do a CS at the machine origin. Then load each tool and set the height using SL,# while the setting tool is on the bed. Then define the part origin Z, and subtract off the difference from the SL,# entries. Pro's is that it is convenient to have a measurement off the bed. Con is that one has to subtract off for each tool.

2nd Approach:
Do a CS at the machine origin. Then set the height off the part as above. Pro is that no subtracting is required. Con is that some of the parts aren't metal and the face setting must be done with a paper slid between the part and tool.

3rd Approach:
Set the SL,# as in the 1st approach. Then measure the difference between the SL,# height and part height, set up a fixture offset and use Exxx to account for the difference.

Of the 3 methods tried, the 3rd seems the best for the way the part is programmed. A SETX & SETY is taken per the part drawing origin, and Z0.0 is 1.00 inch above the part.

What other methods do others use for compensation for height changes between two or more tools? Are there better methods for moving between the machine coordinate system, tooling coordinate system, and fixture offsets?

Thanks.

[little bubba]

Wow, you're really making life complicated for yourself. What controller are you using, on the HS, there are some fantastic simple utilities for setting tool heights and offsets.

Tool heights, if always using a bank of tools that seldom change, I would set all heights to a common height and then use a Z in a fixture offset.

I'm always changing tools, so I usually set my Z zero to the bottom of the part, or the step in the jaw, or the base of the fixture plate, that way I can quickly and easily run several different height parts without changing offsets. I like to program bottom up, some people don't like that, or aren't comfortable with it.

As for the paper to set tool heights, I personally don't like it. You say you are only doing it on plastic, so you are probably safe, but I like to keep the tool away from anything solid when its not cutting, I've seen too many chipped corners from a little slip (stupid operators). I like a 1" gageblock, and if the Z is moving negative, the block is out of the way.

As for the SetX and SetY, you don't need them, you have fixture offsets use them. SetX and SetY are for setting your machine's home position, not for setting fixtures. There are some great utilities for setting fixture zeros also.

I keep my home position at the CS, and have my post configured to return the table to close to the Y+ limit and X0 to gain easy access to the table at the end of a program. I also keep 3 vises and the left hand corner of the fixed jaw, (without jaw) of each vise is E21, E22, E23, all with the same Y coordinate. This makes life easy in so many ways. A lot of times my zero has nothing to do with the part, but is off over there at the corner of the vise.

Also dialing them all in to have the same Y coordinate is a no brainer for me. I seldom have to remove the vises, since they are D688s and I can grab an 18" fixture plate easily, and both of my machines have the extended Z, so I can grab an angle plate in a vise and work on a part that is over 14" tall, above the top of the vises with ease.

[Delw]

wow too much thinking on this one.

simple waywhen using all vise's. touch all 21 tools off the vise jaw locating face, that is zero, then just change your e z offset to what the thickness of the part is.
I have 15 other tools that I use for special stuff, like a few boreing heads, big dia drills 11 endmills a few types of face cutters. they all get seperate tool offset numbers like 22 23 24 25 etc etc. if your worried about screwing up, the just put it in the tool slot you want and set the tool( push the number 5 then yes and your done)

for fixtures that I normally dont run or off the wall parts that dont fit in the vise they get different "E" numbers

all your x and y's will be the same from tool to tool why would you want then different.?

I have 4 kurt vise's set up in my 40x20 with extended jaws the left of each jaw is exactly 9" from vise to vise all the y's are the same

my vice numbers from right to left is E1 E2 E3 E4
if I use all for vises for 1 part in each vise I use E11

sometimes I have3 parts in each vise. I still use E11 .
make sence for me cause everything I do is via a cad cam program., my vise's are already fixtured in my cad cam program.
If I have to replace jaws I make sure I run the program from cad this way I have no problems.

I think bubba and I have pretty much the same set-up except I never use hard jaws always cutable jaws ( mild steel and alumin.). that way everything is perfect from the cad software. to the part program.
less screw ups.

[little bubba]

Originally Posted by Delw I think bubba and I have pretty much the same set-up except I never use hard jaws always cutable jaws ( mild steel and alumin.). that way everything is perfect from the cad software. to the part program. less screw ups.

Guess I said that wrong, my zeros are on the fixed corner of the vise if you took the jaws out. All my soft jaws, or at least the ones I normally use are all 1" thick, so its really easy to figure out. I keep the table mapped in a cad file.

Its a dream set up for me. Where I used to work, most of the vises where different, most didn't work, I had one job that I had to strip the vises off about once a week to run. Now that that job has migrated back to me, me and my partner invested in a fixture that sits nicely across 3 nice new identical vises. Saves a TON of time. Its a tall part so the extra 8 inches of Z certainly helps. Best thing Fadal ever did, I have no idea how I ever lived with only 20" in Z, especially with a carousel sitting out there.

[Delw]

my soft jaws are 1.250 wide I always leave a .500 tab.
I down loaded the dfx files from kurt for the vises I got and put them on my cad system alone with the table slots and pretty much everything.

the upper left corner of my softjaws are 0,0 om each vise.

it took me a year of running parts on that one machine to figure out how I wanted to set it up to be efficient. ( at least for my jobs)

I can pretty much set up any job off the street( the ones I get) in a matter of seconds by just changing the "E" hieght offset. I set it up that way incase something ever happened to me my, wife or daughters could run the machines. my 8 year old is pretty good with it. she has to use a chair to set offsets though LOL. I was thinking of getting her that movable control to make it easier. she uploads programs to the fadal ( saves me from walking LOL)
All the programs have the "E" height amount that should be set before running followed by a "did you set the thickness of the material using the df command" ,msg. with one M00 on that line.



I wish I got a extended z this time around, my next fadal will be a 50 or 60inch one. I like to have the machine run lights out when I for for the day.also want to run 5axis again thats fun.

bottom line is everyone has there own way of setting up a machine, what ever works so they dont make mistakes.

[jon_fallon]

Many thanks for the description of the setups (I'm still getting my feet wet on CNC machining). It is a 1987 4020 w/original controller.

Most of the work to date has been large flat plates cut with a single tool, or drilling hole patterns in large carbon-epoxy laminates. Plastic & laminates are edge clamped on top of a sheet of 1.00 melamine that is slightly larger than the part. SETX,Y&Z have been used to set the part coordinate system to match the drawing.

Defining a fixture offset from the CS position seems the easiest way to use multiple tools. All of the programming to date is being done by a program under development and will include the "did you set the right FO???" in the header line. In thinking about it, programming from the bottom up seems to have its advantages.

How do others fixture large plates? Do you clamp large metal plates directly to the bed, or space them up by a set amount?

[Delw]

Programming from the bottom up does have a bunch of advantages, how ever there is one Major disadvantage.
That is if you have a part that sets 6" high above your table and zero off your table, so the "E1" height is set at 6" your machine z axis will raise up 6" to adjust for the offset before it touches down on the part.


it really comes into problems when you are running long drills and reamers. and you have a 8" part sitting on your vise jaws.