What's new
What's new

Roughing and finishing tool offsets

tmal

Plastic
Joined
Jun 4, 2018
Hi i am new so this may be a simple question. However when I watch videos of setting tool offsets for a cnc milling machine they all show how to set the tool offsets on finish (sides/top) of parts. My question is how to allow for Roughing? If you put a part that is from stock material in a machine and touch off your tools how will you know the finish surface for your finishing tools without re-touching off tools. If I touch off the Z and save the offset, but .010 needs to come off the top of the part with a shell cutter or fly cutter, how can End Mills know the exact top of the part after the fly cutter runs. Is it possible to put rough stock in a machine and have it roughed-in and finished with the same program? I imagine if you have 10,000 parts to run then there must be of way of not having to square-up parts first. I did see a video about using the tool length wear in offsets but don't completely understand it. I want to know the standard way you guys put in rough / oversize material in a vice (against a stop) and do all the roughing and finishing with the same program and how to set the tool lengths and X, Y, offsets to do this. Thank you, and if I am not being clear enough with the question please tell me.
 
Ok this is not as simple an answer as you might like... and I am sure other do things differently, positively, but hope you understand.

So on the tool heights. You need to set all your tools up to a known datum. So some guys will use a tool pre-setter, an in machine probe, the top of their vise, the top of a square block etc etc to get the difference in height offsets for each tool.

Let's say you are touching tools of in machine on a square block. You could either have a master tool that always has it's height offset as 0.0 or you could use a block and know exactly how much lower or higher it is compared to your part. Either way you touch off each tool and get the difference in heights and input them in your offsets page.

Then let's say you went the master tool route. You take your master tool and touch it off on your part. Let's say as in your example you want to take a face cut. Once touching your master tool off you move it down the amount that you want to face and use that as your Z0.0 in your work co-ordinate page. You program your facing at Z0.0 and all tools will work from Z0.0 then.

On the X,Y side you just program your roughing to leave for finish. Then rough it out and either coming back with the same tool or your finishing tool programmed to on the size. You could also use tool radius compensation in your finishing cuts to compensate for the final size you want. No need to use it for roughing, just the finishing. google G41/G42 for Cnc Mill.
 
You could also touch all your tools right off the top of the raw stock then drop your work offset z how ever much to clean the top(.02)
for x and y move your datum 1/2 the amount your stock is oversize(if your datum is coming from a side rather than center
 
I wouldn't really recommend the 'master tool' option though.
Relatively setting all your tools to one tool is fine if your going to break them all down again after that job, but if you plan on leaving them in the machine carousel then absolute length setting to the spindle is much safer.
If your 0 length tool gets nudged, changed, etc, you'll have to reset every tool length.
 
I wouldn't really recommend the 'master tool' option though.
Relatively setting all your tools to one tool is fine if your going to break them all down again after that job, but if you plan on leaving them in the machine carousel then absolute length setting to the spindle is much safer.
If your 0 length tool gets nudged, changed, etc, you'll have to reset every tool length.
Agreed to a certain extent. For production your thought train is spot on because changing out tools would be loads easier... especially if you use a few of the same tools for different parts.

The way I use a "master" tool is a bit different. I am more of a jobbing shop so don't often do long runs on parts. My master tool varies with each part. So on one part it could be a spot drill and on the next it might be an inserted endmill, honestly it is usually the tool that is first in my hand when I am loading tools. I don't care where my Z work offset is from any particular point on my machine because I am constantly switching from vises to chucks to the 4th axis to the table and so on.

Your point is valid though, if something happens to your master tool during a part you either have to check what the new difference in length is from the old one or you could also just load a new tool and touch it off and give it an offset relative to the old tool and run the part without even having set a new master tool.
 
I've done the "master tool" thing too in the past, although I don't recommend it either. What I did that made the other tool lengths more stable was to use something that doesn't vary (like a face mill) for your master, whether you're using it on this job or not. Twiglet's idea is better.
 
I use a 3d taster as my master tool. Set all my tool lengths as the difference between the tool and 0 on the taster. That way all I have to do is touch off the part with the taster for my Z zero and all the tools follow along.

Teryk

Sent from my XT1710-02 using Tapatalk
 
First: Thank you and all who replied!

I understand touching the Z's off from the back of the vise or the work table and then using G54 to offset the machine's absolutes difference from the table/vice+(1-2-3 block) to top of the part and making it G54's zero and it should work on all the tools Zs if all the tool offsets are touched from the same standard like table + gage.

Then would it be acceptable to add a positive .010 value in G54's Z's WEAR to allow the roughing and then adjust the WEAR down for finishing?

Also for X and Y, if Stock material is in the vise (back left and top of part the origin) would you even need an edge finder? I would think using an edge finder would only be good for setting X and Y on finish sides.

I think I understand what you are saying about setting the fly cutter tool offset up and then move it down ten thousands and making that Z's zero. So as long as you are not setting off the top of the part then all the other tools can use the zero from the face cut?

Tool Offset.jpg

In this crude drawling when I touch off the 2" side of the 1-2-3 block the machine's Z reads -18.000" so in the offset page under the tool number I'm using, I hit tool offset measure button then with same tool selected go to command and type -2.000 enter or (+ -2.000) which allows for 2" block/standard that will set the table at -20.000 machine absolute. Next I would hit the offset button 2x and under G54 enter 10.010 in Z (please correct me if I am getting this wrong especially what to enter in as negative or positive offsets so Z won't crash)

Or, should I enter in just 10.000 in G54 so to allow for roughing?
 
Last edited:
Generally you would program your roughing at z+.01. That way you don't have to adjust offsets. In general, offsets are more for setup purposes. Programmed points determine the motion of the machine.

As for X and Y (and Z), it depends on how you setup your zero. My last shop liked putting the zero at the center of the part in X Y and top of rough stock in Z. My personal favorite is to program around the bottom, back, left corner of the rough stock and have the program compensate for this (makes it easy to swap programs/stock).

The zero point is just a "known" point in space. you can put it anywhere and then compensate via your programmed points relative to it. If you really wanted to, the zero could be outside the machine and still produce good parts.
 
First: Thank you and all who replied!

I understand touching the Z's off from the back of the vise or the work table and then using G54 to offset the machine's absolutes difference from the table/vice+(1-2-3 block) to top of the part and making it G54's zero and it should work on all the tools Zs if all the tool offsets are touched from the same standard like table + gage.

Then would it be acceptable to add a positive .010 value in G54's Z's WEAR to allow the roughing and then adjust the WEAR down for finishing?

Also for X and Y, if Stock material is in the vise (back left and top of part the origin) would you even need an edge finder? I would think using an edge finder would only be good for setting X and Y on finish sides.

I think I understand what you are saying about setting the fly cutter tool offset up and then move it down ten thousands and making that Z's zero. So as long as you are not setting off the top of the part then all the other tools will can use the zero from the face cut?
Hmmmmm,
So I would not do it like that. What if you wanted to run more than one part? Offset the first one in Z then offset again for the next to rough and then finish? I suppose you could but it could lead to you forgetting the second step and running it without setting back up. Your tools should be set, in my opinion, correctly in Z from the get go. Teryk's method seems the same as a "master tool" but it will land up being pretty much dead nuts because of the use of a 3d taster.

I think you are confusing yourself. Once your origin is set it does "should" not change so all programming, whether it is roughing or finishing, does not move from the origin. Put your part in, set your origin, write your program with known stock size, leave for finish.... offset if needed.
 
the roughing allowance is in your program. Has nothing whatsoever to do with how you set your tools.

This is the way to do it......................set all your tools off on a common Z(vise, table, 123 block, toolsetter). Use one tool to touch off on the work, adjust for clean up on the stock, and hit the green button.
 
I use a 3d taster as my master tool. Set all my tool lengths as the difference between the tool and 0 on the taster. That way all I have to do is touch off the part with the taster for my Z zero and all the tools follow along.

Teryk

Sent from my XT1710-02 using Tapatalk

This is a good idea.
Master "tool" need not be a machining tool.

Another way can be, as suggested by NAST55, to keep another master tool, with the difference in the length from the original master tool be known. With the new master tool, the work offset can be appropriately edited.
 
This is the way to do it......................set all your tools off on a common Z(vise, table, 123 block, toolsetter). Use one tool to touch off on the work, adjust for clean up on the stock, and hit the green button.

And walk away, or alternatively keep your butt hole connected to the feed hold so that if it clinches the tool doesn't bury itself in the crazy abyss that i like to call the "WTF HAPPENED SYNDROME ZONE"
 
First: Thank you and all who replied!

I understand touching the Z's off from the back of the vise or the work table and then using G54 to offset the machine's absolutes difference from the table/vice+(1-2-3 block) to top of the part and making it G54's zero and it should work on all the tools Zs if all the tool offsets are touched from the same standard like table + gage.

Then would it be acceptable to add a positive .010 value in G54's Z's WEAR to allow the roughing and then adjust the WEAR down for finishing?

Also for X and Y, if Stock material is in the vise (back left and top of part the origin) would you even need an edge finder? I would think using an edge finder would only be good for setting X and Y on finish sides.

I think I understand what you are saying about setting the fly cutter tool offset up and then move it down ten thousands and making that Z's zero. So as long as you are not setting off the top of the part then all the other tools can use the zero from the face cut?

Sounds to me like you're making aMountain out of a Mole hill. It's really not that big of a deal, and it will become painfully obvious when it's wrong. It is a reality that a lot of this learning curve is making mistakes and learning from them.

ULTIMATELY; it doesn't matter, you could set your Part zero anywhere you want, as long as the Program matches it. You could set your Zero's at Home Position (which I have seen, and would never recommend). Process planning is what this is called.

If you are the programmer and the newbie, keep it simple. Drop a chunk of material in a vise, find XY zero in the middle of the material, touch all your Tool lengths off of whatever the hell you want. Then go Program the part based on that information, and know that the height can be adjusted in the Work, Wear or Geometry offsets. OR program first, then set it up the way it is Programmed.

R
 
If I touch off the Z and save the offset, but .010 needs to come off the top of the part with a shell cutter or fly cutter, how can End Mills know the exact top of the part after the fly cutter runs.

If you are going to skim .010" off the top of your part you can either 1) touch all of your tools off to the rough top of your part and then manually add in the .010" to their respective length offsets or 2) one way or another get your part to the exact right height and then touch all your tools off to that surface. Then you program your skim cut to be at Z0. and all your other depths to be programmed relative to the top of your finished part (likely as shown on the print). So instead of programming a 1" deep hole to "Z-1.01" you get to program "Z-1."

I typically do #2 and then saw cut material to whatever length is required for an appropriate cleanup facing op. So if I need a 1" finished height to my part I may saw cut to 1.025", thus providing about .025" worth of material for facing with the programmed facing op at Z0. Good luck!
 
Are you a student????????

I used to run a Bridgeport with Proto Track and servo motors fitted with glass scales. I'm trying to teach myself how to run a HAAS CNC machine. So i know the basics of machining actually much more then basics. Back then things were a lot harder:

Tramming machine, putting cellophane shims around tool in the collet and indicating the tool spinning true, double sided taping parts, vacuum plates, running endmills in hole to get better true position, grinding my own drills to resharpen them, stoning custom radii on endmills, using the knee for better tolerance, machining soft jaws, making my own fly cutters, 1-2-3 blocks, stops, and heat treating to case-harden my made tools, etc. Worked at a prototype aerospace shop with tolerances in the tenths. but this was all with DRO's as are best technology lol.
 
Sounds to me like you're making aMountain out of a Mole hill. It's really not that big of a deal, and it will become painfully obvious when it's wrong. It is a reality that a lot of this learning curve is making mistakes and learning from them.

ULTIMATELY; it doesn't matter, you could set your Part zero anywhere you want, as long as the Program matches it. You could set your Zero's at Home Position (which I have seen, and would never recommend). Process planning is what this is called.

If you are the programmer and the newbie, keep it simple. Drop a chunk of material in a vise, find XY zero in the middle of the material, touch all your Tool lengths off of whatever the hell you want. Then go Program the part based on that information, and know that the height can be adjusted in the Work, Wear or Geometry offsets. OR program first, then set it up the way it is Programmed.

R

Fine, so long as "touch all your Tool lengths off of whatever the hell you want" stays in existence. If you machine the touch off surface to flatten a piece to create a Z0, then you have destroyed the reference. I've mentioned this before, but I 'fell out of love' with touch off of whatever the hell you want one time when I was doing surfacing of a mold, a program that would run for a few hours. I broke a tool, touched off the top of the part (which was no longer the reference surface) and proceeded to waste a few hours until I found that the new tool was cutting at a slightly different depth than the old one. So then I had to remachine the surface a third time to get a proper blend.

I used a tool setter block religiously ever afterwards. Use an unchanging reference at all times for tool setting because it will bite you when you least expect it.
 
All of my tools are zeroed on a 2" height gage, on the table.
That way I only have to set tool heights 1 time.
Why would anybody retag EVERY tool on each setup?:confused:

Call up any good tool and touch off the part. (either by way of height gage, or a piece of paper)
~~~~~~~~~~~~~

As stated above, the amount of material to remove (roughing allowance) has nothing whatsoever to do with tool offsets between respective tools.


Doug.
 








 
Back
Top