What's new
What's new

proper way to set z height for face milling rough cut parts

garychipmaker

Cast Iron
Joined
Dec 2, 2005
Location
ia
What's the proper way to program Z height for face milling when parts are saw cut varying in height by .500". Program first cut as a Z+ height and take air cuts possibly working to Z 0 . Or setting Z 0 high enough to take cuts progressively to a Z- number. Part is 4.5" finish height. part will be flipped over after a face mill pass and 8 holes drilled and tapped.
 
What to do with varying incoming stock?
One is program at the max and spend some time cutting air.
Other is to probe and do some fancy programming.
Think this one. PCD tool tip brazed on. Hand positioned. This stuff does not like to be ground at speed.
I have .010 or more variation coming in. Grind infeed is .002/.004 per minute at the rough op.

Can anything be done to control the saw cut height tighter?
 
Last edited:
Air cutting the safest method. Program multiple depth cuts for the thickest possible stock size.

You can also probe and face with a macro counter, eliminating all air passes, but you'd need a decent quantity requirement to justify the hassle.
Or just go maybe .450 deep on the first pass on tall parts. What could go wrong? :D
 
Parts are saw cut out of a very large slab of copper 300Lbs with a very large bandsaw. Saw table has a crude power table and they have no desire to cut my parts to any accuracy. 5 sides are saw cut. Sometimes parts are cut an Inch oversize 1 dimension and with .250 another with none of the 6 sides reasonably square with another side, FUN, We are getting a VMC to run these on. we did these on a HBM before.
 
You can also probe and face with a macro counter, eliminating all air passes, but you'd need a decent quantity requirement to justify the hassle.
That is the real key here. Time lost cutting air vs time and money spent coding a probe and cut program.
Attended or unattended? Is the machine tool a bottleneck or does it have lots of free time doing nothing?
 
Cut first one.
Measure height.
Set a variable at the beginning of the program and use IF THEN and GOTO statements. If stock is 10mm higher than finish measured with rule program starts at Z+10 if 5mm starts at Z+5.
 
Cut first one.
Measure height.
Set a variable at the beginning of the program and use IF THEN and GOTO statements. If stock is 10mm higher than finish measured with rule program starts at Z+10 if 5mm starts at Z+5.
 
What's the proper way to program Z height for face milling when parts are saw cut varying in height by .500". Program first cut as a Z+ height and take air cuts possibly working to Z 0 .
0.5" is a fairly poor result even for a rubbish saw. I would be trying to improve that for a start.
However, the following is a simple Macro solution to accommodate the height variation when machining, but you would still have to first either sort the blanks into similar height groups or use some method of probing the top surface of the part.

G90 G00 G54X_ _ Y_ _
G43 Z0.75 H01 M08
#1 = 0.50 (Z START POINT)
#2 = -0.125 (DOC)
#3 = 0.0 (Z FINISH POINT)
WHILE [ #1 GT #3] DO1
#1 = #1 + #2
IF [#1 LT #3] THEN #1 = #3 (STOP OVER CUT IN Z)
G01 Z#1 F_ _
-------------------
-------------------
FACING CODE GOES HERE
-------------------
-------------------
END1

Only the value of #1 needs to be altered to accommodate the varying thickness blanks. A Probe could be used to do that, or if the machine is not so equipped, provide an M00 just after the G43 Block then manually move the Z Axis down until the Face Mill just clears the top surface of the part. Macro Code could be included just before the #1 Block where the Z START POINT is set, so that when Auto Mode is again selected and the Cycle Start button pressed, the #1 Variable will be set to the current Z Absolute coordinate.

Regards,

Bill
 
I've had some wonky cut 7" round bar aluminum that sloped up 1/2
" or so (wonky stock cut by me and my clapped out band saw). I set my WCS at the bottom of the stock, haul ass with adaptive roughing 1/2"x1" loc serrated rougher leaving .01 of stock for the face mill path. I set my roughing F&S for the max height deviation expected from the wonky stock. My "production" maybe ~20 parts, so maybe not the fastest method, but I can load and walk away without fear of jamming the face mill.
 
Like how everyone always gets off on a tangent from the questions. their better mouse trap.
To answer the OP question, most machinists I know program to the top of the finished part, main reason I do this is easier to setup clearances, but mostly because, then when looking at gcode all the depths are the actual depths,
I don't need to sit there with a calculator during first article to know if something was right or wrong, just look at it, yep, and keep going.
So when there is a lot of material to remove from the stock before I can start all of the other machining, I program Z 0 at top of the finished part,
in your case a (+).6 clearance, (+) .5 starting height, coming down to Z 0 for the finish.
 
This also how to spot a Youtube trained machinist, they like to set their z zero on what ever they are setting the part on, jaws, parallels, fixture...they like to put Z Zero on the bottom of the part.
That's why you see them crashing their machines all the time, haha
 
I don't want to say too much about our part to get in trouble at work. I should have worded it a bit different. the part weighs 300 Lbs. rough cut. about 9 x 5 x 31". the saw usually cuts straight to within a 1/16 -1/8". the clamping of the part when sawn is the problem. They have no desire to make the setup better and we make only about 20 a year. Yes if the saw operator would spend 5 minutes more time It would save me an hour of time. sometimes the ends are cut like a parallelogram and so close to finish size that it has to be setup for the first cut at an angle on the long side so it will end up square to the ends. about like working on an old house where nothing is square. The clamping setup on the saw isn't the best as it's meant to clamp a 22 foot part. We produce the bar and re melt the scrap so the chips aren't waste.
 
Personally I would keep it simple and just batch the parts. Program your passes for the tallest stock at z+.500 and machine to z 0.

Once the first batch is done, delete a z pass and then run the next batch. Repeat until all are done.

This is something I have done plenty if times.

This also depends on quantity run and who is operating the machine... I would not let an simple operator do the program mods unless they are experienced enough to trust with first runs at low rapid.
 
Personally I would keep it simple and just batch the parts. Program your passes for the tallest stock at z+.500 and machine to z 0.

Once the first batch is done, delete a z pass and then run the next batch. Repeat until all are done.
I love probing and macros, but for 20 parts per year? I'd do the same as Turntech.
 
Another twist in the story is this is going to be run on our first CNC machine in the shop which is supposed to arrive this week. Its' a Prototrak TMC .I have a Fadal 4020 at my personal shop .Night guy has experience with a Prototrak . He thinks about as opposite as I do on anything so That's always fun LOL.Other guy hasn't run a CNC for over 15 years. the part has threaded holes, chamfers and dovetails cut into it at an angle so it's 13 different times of flipping and rotating the part on the HBM we now use. The copper is almost a thing of beauty when finished. My thoughts are to maybe take a pass on the large face and a skim cut on the 2 long sides to start with to have something to hold onto in the VMC. But it takes time to clean the HBM to make sure we don't contaminate the copper chips with steel.
 
It takes 8-9 hours a part to do these on the worn out G&L. Ways are so worn part has to be shimmed to cut square. This machine is what I wanted replaced. So the VMC will be able to do this in 2 setups hopefully. We do mill to size all the batch then do all the holes and then the all the chamfers etc. oh I forgot it has radiused corners too so 2 setups for the 4 radiuses
 
Parts are saw cut out of a very large slab of copper 300Lbs with a very large bandsaw. Saw table has a crude power table and they have no desire to cut my parts to any accuracy. 5 sides are saw cut. Sometimes parts are cut an Inch oversize 1 dimension and with .250 another with none of the 6 sides reasonably square with another side, FUN

I know it is easier said than done but I would address this issue first. If they are that sloppy, you will never get +1/16" out of them. However, if they could at least maintain 1/8"-1/4" extra stock, it would be better than what you have now.

Next, milling these...
1st, I would set your Z 0.0 on the top of the parallels and program the cut depths as Z+. It is much better this way because your program will show the actual target dimension, rather than just the DOC from the top of stock.

Since you have so much extra stock, I would not face all 4 sides, that takes a lot of extra time. I would clamp the bars in a vise, only holding onto the excess stock. I would then face the top and use a contour tool path with an endmill to cut the other two faces and the ends of the bar. Cut everything right to size and square in one go. You can even run a chamfer mill to deburr - I'm sure you're well aware how much it sucks to deburr copper by hand.

Finally; flip the bars upside down, clamping on what you've already machined and face the extra material off the top. Run the chamfer mill again and remove your finished bar.

If you set up 2 vises, you can do op1 and op2 in one cycle. Raw stock in, finished stock out.
 








 
Back
Top