[mnicholas77]

I've been pulling my hair out, what's left of it, over the fact that I can't nail a part thickness in Z to save my f'ng life. I use a Edge Technologies Z tool offset tool (4.000" tall) to set T0 (no tool in spindle), touch off the spindle nose until the gauge reads zero. I've set my Haimer T50 a few different ways in an attempt to figure out why my parts are always like 7-15 (.007-.015") thou off. I have accurately adjusted my Haimer tip within a few tenths of concentric and have adjusted the gauge face glass cover so that when the probe isn't touching anything, I've got the long hand reading zero. At first I touched my Haimer off to the offset tool, but quickly realized that the Haimer probe won't compress to zero because the offset tool isn't stiff enough to resist the Haimer until it reads zero. Then I removed the Edge Technologies tool offset holder and replaced with a 2-4-6 block, then touched off my Haimer until the Haimer read zero on the 4" part of the 2-4-6 block to simulate the 4" from the offset tool. The Haimer will then accurately measure distance in the Z direction. So then when I machine a part, doesn't matter if I'm using a stock reference point or model reference point in Fusion, I can't make an accurate part in Z height to save my life. I really don't understand what I'm missing and have been frustrated for months trying to figure out what I'm screwing up. Any ideas?

[Gerry Kmack]

When you set zero on your offset tool, make sure that the collet is removed or retracted. If you have a PDB, and the spindle is in the "open" position, the collet will be protruding below the spindle nose. Don't ask me how I know this


Sent from my iPad using Tapatalk

[upnorth]

Have you confirmed with the 2-4-6 blocks that your edge technologies tool setter is actually at zero when it is reading zero?

[joshetect]

The Haimer has to make 2 rounds to be zero.

I'd take the Edge Technologies tool out of the equation. touch the spindle off of your 246 block, zero, then put the Haimer in and touch off the 246 block. Now see how well the Haimer repeats. If its ok, I'd think your problem lies with the ET height gauge.

You can also check the ET z height with the 246 block to make sure its reading ok.

[mnicholas77]

Thanks Gary. Yeah I always make sure no collets, chips or anything else is contacting the offset height tool except the spindle. I can't help but think it has something to do with the travel inside the Haimer itself? I mean what else could it possibly be. I will say this though. Yesterday I had internet issues with sending my post from Fusion to my Tormach mill. I always choose "open guide in editor", so this one time K copied and pasted the actual code from Brackets (g code text editing application)to USB and then copied the the text to Path Pilot. My part z height was a lot closer then it previously ever had been, about .0035", but I'm not sure why. I'm not trying to hold tenths but 3.5 thou still seems like a mile away.

When you set zero on your offset tool, make sure that the collet is removed or retracted. If you have a PDB, and the spindle is in the "open" position, the collet will be protruding below the spindle nose. Don't ask me how I know this


Sent from my iPad using Tapatalk

[mnicholas77]

Yes, I use the 2-4-6 blocks to set my 4" height on the touch off tool.

Have you confirmed with the 2-4-6 blocks that your edge technologies tool setter is actually at zero when it is reading zero?

- - - Updated - - -

I'm going to try that next. I do calibrate the touch off tool to my 2-4-6 blocks though.

The Haimer has to make 2 rounds to be zero.

I'd take the Edge Technologies tool out of the equation. touch the spindle off of your 246 block, zero, then put the Haimer in and touch off the 246 block. Now see how well the Haimer repeats. If its ok, I'd think your problem lies with the ET height gauge.

You can also check the ET z height with the 246 block to make sure its reading ok.

[mnicholas77]

I do make the Haimer make two rounds til both pointers are at zero.

The Haimer has to make 2 rounds to be zero.



I'd take the Edge Technologies tool out of the equation. touch the spindle off of your 246 block, zero, then put the Haimer in and touch off the 246 block. Now see how well the Haimer repeats. If its ok, I'd think your problem lies with the ET height gauge.

You can also check the ET z height with the 246 block to make sure its reading ok.

[mnicholas77]

Yes, I set the tool height gauge with 2-4-6 blocks. I set one block on its side for a 4" height on a granite surface plate and then place another 2-4-6 block on top. Then I slide in the offset tool gauge and dial bezel into zero with the top block pressing on the tool pad.

Have you confirmed with the 2-4-6 blocks that your edge technologies tool setter is actually at zero when it is reading zero?

[joshetect]

so two things

In fusion, for each CAM op there is a setting for accuracy. Make sure that is set to lower than you need. mine defaulted to .004 !!

The next thing you can do is check your backlash for x,y and z. Then you can set that in Path Pilot to adjust for it. Although Z should hopefully be way less than you are seeing. But worth checking

[C*H*U*D]

...I use a Edge Technologies Z tool offset tool (4.000" tall) to set T0 (no tool in spindle), touch off the spindle nose until the gauge reads zero.

I don't really understand this part of your procedure. Why are you worried about setting the spindle nose as tool zero? Is this just part of your troubleshooting or do you do this for every part?

I have accurately adjusted my Haimer tip within a few tenths of concentric and have adjusted the gauge face glass cover so that when the probe isn't touching anything, I've got the long hand reading zero.

The important thing is that you have the correct length offset entered when you have the dial compressed to your zero mark.

Then I removed the Edge Technologies tool offset holder and replaced with a 2-4-6 block, then touched off my Haimer until the Haimer read zero on the 4" part of the 2-4-6 block to simulate the 4" from the offset tool.

So are you referencing the 4" from the table, the vise or the part? I guess I don't understand why you are using two different tools to do your measuring. The Haimer just needs to touch what you're working on. Or is this also part of your troubleshooting? I use a Haimer at work, but at home on my Tormach I use a dial indicator for Z which works exactly like a Haimer would (I just don't have X and Y). To get accurate Z heights, I measure off of the bottom of the part so that means I measure to the parallel, soft jaw or whatever is going to be touching the bottom of the part. In Fusion I set my CAM origin on that bottom surface as well. My Z height is actually my most accurate out of the three on my 770, and I usually hit it within .0005".

The Haimer will then accurately measure distance in the Z direction. So then when I machine a part, doesn't matter if I'm using a stock reference point or model reference point in Fusion, I can't make an accurate part in Z height to save my life.

So if the Haimer is accurately measuring distances in Z, but your machined parts are wrong, then something in your procedure is to blame, not the Haimer correct? Sorry if I'm confused, I'm just trying to understand your procedure better.

[LeeWay]

I do make the Haimer make two rounds til both pointers are at zero.

Both pointers read zero when the Haimer is at zero.

[joshetect]

So are you referencing the 4" from the table, the vise or the part? I guess I don't understand why you are using two different tools to do your measuring. The Haimer just needs to touch what you're working on. Or is this also part of your troubleshooting? I use a Haimer at work, but at home on my Tormach I use a dial indicator for Z which works exactly like a Haimer would (I just don't have X and Y). To get accurate Z heights, I measure off of the bottom of the part so that means I measure to the parallel, soft jaw or whatever is going to be touching the bottom of the part. In Fusion I set my CAM origin on that bottom surface as well. My Z height is actually my most accurate out of the three on my 770, and I usually hit it within .0005"..

He is using the Edge Tech as a tool height setter.It setup so that you can check its accuracy with a 4" gauge block

Pro Touch Off Gage - Edge Technology

[LeeWay]

That is how I use both of those tools and it is pretty accurate for me. After a weeks worth of machining on the Haas mini mill, I had about a .0002" difference in the readings.
That could be in the home switch.

[mnicholas77]

I am setting my T0 (empty spindle) at an arbitrary zero (using offset tool height gauge) in order to reference all of my tools for a total tool height (procedure in Tormach owners manual, except using a 4" height gauge instead of .003" paper). Usually I'll set the tool offset gauge on top of a ground surface like my vise (not on jaws or while under tension) depending on how I have the machine setup for task at hand. All of my tool offsets come after setting my spindle nose to zero, then setting total tool offset (ER collet holder and tool combined).Once my tool offsets are set (including initial setup of my Haimer T50), then of course I set my work origins. Depending on my part, sometimes in Fusion I'll set up my work origin from "stock point" or I'll use "model point" depending on what I'm doing...ie I'm likely to use stock box point for OP1 and then use model box point for saying locating and decking the back side OP2.

I don't think the Haimer is to blame either, I can get it to repeat from a set zero to a known gauge block height, and back to zero. This is the exact reason why I'm loosing my mind. I'm going to try to eliminate the Edge Technologies height gauge, but I honestly don't see how that could be the issue. The issue is seemingly the relationship between the Haimer "zero" and my tool and/or work offsets. I just don't know what it is.

I don't really understand this part of your procedure. Why are you worried about setting the spindle nose as tool zero? Is this just part of your troubleshooting or do you do this for every part?



The important thing is that you have the correct length offset entered when you have the dial compressed to your zero mark.




So are you referencing the 4" from the table, the vise or the part? I guess I don't understand why you are using two different tools to do your measuring. The Haimer just needs to touch what you're working on. Or is this also part of your troubleshooting? I use a Haimer at work, but at home on my Tormach I use a dial indicator for Z which works exactly like a Haimer would (I just don't have X and Y). To get accurate Z heights, I measure off of the bottom of the part so that means I measure to the parallel, soft jaw or whatever is going to be touching the bottom of the part. In Fusion I set my CAM origin on that bottom surface as well. My Z height is actually my most accurate out of the three on my 770, and I usually hit it within .0005".



So if the Haimer is accurately measuring distances in Z, but your machined parts are wrong, then something in your procedure is to blame, not the Haimer correct? Sorry if I'm confused, I'm just trying to understand your procedure better.

[joshetect]

See my post above about the accuracy setting in fusion

[mnicholas77]

I will triple check that setting, but I am aware of it and have used smoothing or adjusted tolerance down to .0004" instead of 4 thou on tool paths that make sense. Even at 4 thou, there's no reason why I can't get a 2D part to within +/- a thou or two with one setup change, but I'm getting like 10-12 thou. Parts are relatively flat, just not to thickness. Someone mentioned adjusting for backlash in Fusion, but I'm not quite sure how I'd do that. I do have some back lash but I'm able to repeatedly (like 20 times up and down) be within a couple tenths when using the Haimer and 2-4-6 blocks. I just can't get a part to be on thickness. Going crazy and highly demoralizing.

[mountaindew]

Like others Have mentioned above. Set Hamier probe height in tool table. Then set that as current tool number. Move probe to any point on table, vice, 123 block and set probe height to zero after one or 2 full sweeps of dial. I only use one full sweep. Then zero the machine z axis. Move the hamier probe away and then back to zero and look at Z value on PP or other controller interface. My Tormach reads less then 0.0007, even after homing and checking the next day. Simple, unless your using some other system I dont understand.

[mountaindew]

I will triple check that setting, but I am aware of it and have used smoothing or adjusted tolerance down to .0004" instead of 4 thou on tool paths that make sense. Even at 4 thou, there's no reason why I can't get a 2D part to within +/- a thou or two with one setup change, but I'm getting like 10-12 thou. Parts are relatively flat, just not to thickness. Someone mentioned adjusting for backlash in Fusion, but I'm not quite sure how I'd do that. I do have some back lash but I'm able to repeatedly (like 20 times up and down) be within a couple tenths when using the Haimer and 2-4-6 blocks. I just can't get a part to be on thickness. Going crazy and highly demoralizing.

How are you using offsets in cam? I use top of part for first side. Then when I flip the part I use the bottom of part as offset and the cam software mills to that height or part thickness to + - 0.0005
Far beyond my quality of measuring tools to even check.

And as I have noted in other threads. I get best results if I first prep the stock with couple of nice square and or parallel stock faces. In wood working terms its called s2s or s3s. "surface 3 sides" Then when stock is loaded into vise jaws it sets flat and as parallel and square to all the machine axis as possible.



picture example
top of part is milled off and all other ops are performed at that z offset. Note the extra 1/4" stock at bottom of part held in vise.


Attachment 370036

Flip the part over and set the offset to the bottom of part that is the nice shiny face you Just milled off. Have the cam software calculate what the difference is and mill off the top of part. You should have about as precise of height / thickness as your machine can make.


Attachment 370038

[mnicholas77]

In CAM I will usually set my CAD model with stock .020" above the part and set zero for the stock top for setup1/OP1. On the machine I will touch off zero on my stock top (WCS) with the Haimer for OP1 and execute program. Then in CAM for stock setup 2/OP2 I will choose a model point (versus stock point) for zero to locate my part, typically with zero being the top of the CAD part model and X/Y say in a known feature such as a pocket to pick up location for OP2. On the machine, I will touch my Haimer off to parallels or whatever my real life part is sitting on, and zero Haimer (WCS) in PathPilot. Then I will move the Haimer up to whatever my CAD model zero point thickness was, and re-zero my Haimer (WCS) in PathPilot. In other words, if my part model finished thickness is .750", then I will touch off the top of the parallels and zero (WCS) in PathPilot, then move Haimer up .750" in Z and reset zero WCS in PathPilot. Am I flawed in setting up these parts? I know some will choose bottom of part for Z zero, but I've seen plenty use the top of the part as well.

[SCzEngrgGroup]

I used to sometimes zero on the top of the work, sometimes the bottom, but for several years now have nearly always zeroed on the bottom. When I need an exact finished height, I start with over-size stock, and setup the stock in CAM so the top operations to have extra stock on both top and bottom, while the stock for the bottom operations has extra stock only on the top. That way, a single fixture can be used for both top and bottom operations, eliminating a second fixture offset - one potential source of error. This also means I can, if necessary, re-work the top of the part at any time, since I am not dependent on the top stock height to be able to accurately set fixture offsets for the top features. Reducing the number of fixture offsets is one way to minimize errors, and most parts, even when machined on all sides, can be made using a single fixture offset.

Regards,
Ray L.