# Fixturing and toolpaths for noobs



## koenbro (Jul 5, 2022)

I struggle with completing parts, and don't know how to release them from the stock. Consider this part:



It is a simple circular adapter with four holes and a protrusion with a shoulder. Overall 0.5" thick, and working it out of 0.64" thick alu plate. I was able to to the spot drilling, through drilling, and the rest of contours, but then I am left with a piece still attached at the bottom in the stock. What are the best practices to complete the job?

This time I took a crude approach and cut the contour out with a bandsaw then flipped into the vise using the stickout and am going at it with a fly cutter, little by little, but would like to program this (the first face with all the steps was CNC'd). Any advice is greatly appreciated.


----------



## Cadillac (Jul 5, 2022)

Mill off the last .140 after flipping over.


----------



## mmcmdl (Jul 5, 2022)

Are you looking to remove the extra square stock on the bottom ? If so , put it on parallels and mill it off .


----------



## tq60 (Jul 5, 2022)

Should change order of operations.

Fly cut the bottom first to make it flat.

Flip over and place on parallels then do all of the top stuff.

Make to size by removing material.

Sent from my SM-G781V using Tapatalk


----------



## mmcmdl (Jul 5, 2022)

tq60 said:


> Flip over and place on parallels then do all of the top stuff.


If I'm seeing this right , it would be hard to cut that circle if it was down in the vise .  I think his OOO is correct .


----------



## koenbro (Jul 5, 2022)

I would like to avoid the bandsawing part and would like to automate the back side as well. 

So I guess I need to face the stock, both top and bottom, then measure its thickness precisely and input that thickness into Fusion 360 setup as the stock size. Then do the tops size holes and contours, then flip and face the bottom with the flycutter? but then the piece will fly away as it is not supported/held. 



Sent from my iPhone using Tapatalk Pro


----------



## mmcmdl (Jul 5, 2022)

If I was making this . I would start with round stock , face and turn round diameter in lathe . Bore soft jaws for the mill and mill the square , face cut to final thickness and do all your holes . 2 set-ups . Not sure what stock or machines you have , but it's how I would do it if a production run .


----------



## tq60 (Jul 5, 2022)

Looking again at the model it seems like there is a square shape on top that it looks like you are holding it in the vice by.

A lathe would work as well.

Your hold in the vise should be fine.

Maybe smaller cuts.

Sent from my SM-G781V using Tapatalk


----------



## dbb-the-bruce (Jul 5, 2022)

It's not entirely clear what kind of answer you are looking for - do you want to do the entire job with CNC? how many are you making?

I've been teaching myself CNC and I too have struggled with fixing and holding. Considering the part you have, I'd drill the holes and then figure out how to temp bolt it to the CNC bed (bolt hole grid or sacrificial plate). Get some thin ABS plastic sheet (for sale signs etc, at the HW store) and use it to space the stock off of the base by about .030 or so. Set your Z zero to about .002 - .005 below the top ABS surface and you are good to go. The point being that however you set Z over cut the outer most profile/contour a few thou deeper (into the ABS). I usually face one side and flip, remove any extra off of the top.

Make a lot of small 2.5 D parts out of 1/8 or 1/16 brass stock. So I can use double sided tape or super glue to hold the stock. The most reliable I've found is double sided tape the ABS to the base and super glue the stock to the ABS. CNC a slight recesses about .1 deep for stock registration.

This part looks like it wouldn't be that hard to do by hand (with out CNC - possibly quicker if you are only making one). If you have a lathe and/or round stock to start with. Turn the cylinder section and then cut the square stuff into it on a mill (do the holes then to)


----------



## Boswell (Jul 5, 2022)

here is another approach. 
1. use your face mill or fly cutter to clean up one side of the rough cut stock
2. Flip the  part over and clamp to the mill table with a piece of sacrificial MDF between the part and the table
3. Complete the milling of the part. 

Alternately you can put a spacer under the part as long as it does not stick out from under the finished profile. for a small part like this, MDF is probably easiest.


----------



## JimDawson (Jul 6, 2022)

You have 3 counterbored holes in the part, use them.  Use a scrap piece (fixture plate) in the vice. Face it off and drill and tap the hole pattern into the piece.  Clamp the workpiece to the fixture plate, drill and C-bore the holes.  Screw the work to the fixture plate and remove the clamps. Do all the machining from one side.

Rather than facing off the back with a fly cutter, use a 3/8 endmill and take it all in one pass using a facing routine.  Around 2800 RPM, 18 IPM, 60% stepover.


----------



## koenbro (Jul 6, 2022)

JimDawson said:


> You have 3 counterbored holes in the part, use them.  Use a scrap piece (fixture plate) in the vice. Face it off and drill and tap the hole pattern into the piece.  Clamp the workpiece to the fixture plate, drill and C-bore the holes.  Screw the work to the fixture plate and remove the clamps. Do all the machining from one side.
> 
> Rather than facing off the back with a fly cutter, use a 3/8 endmill and take it all in one pass using a facing routine.  Around 2800 RPM, 18 IPM, 60% stepover.




Yeah I like this (and @Boswell ‘s) plan best. I have a LMS fixture plate and can use an MDF piece sandwiched between the Alu stock and the fixture piece. Or remove the fixture plate and attach the MDF directly to the bed.

I use this all the time on the CNC router btw, but was reluctant to use MDF as I think the lateral forces are quite high. 

I think this must come up very often -- what kind of material do y'allz use as a backer?


----------



## JimDawson (Jul 6, 2022)

koenbro said:


> I think this must come up very often -- what kind of material do y'allz use as a backer?



It depends.  Sometimes MDF, sometimes aluminum.

Here is an example of a MDF backer and the parts bolted directly to the table.  The large cap screws use the T-slots, the smaller ones are drilled & tapped into the MDF.  Work material in this case is 1/2'' steel, this started out as one solid piece about the size of the MDF.



Here is an example of using an aluminum fixture plate with the work screwed down to it.  This also has a tooling plate under the the aluminum backer. 



These are the parts that were machined on the above setup



Here is a chunk of 4140 bolted to an aluminum backer in the vice.  Punch press connecting rod.



I have many more examples, but I think you get the idea.   You are only limited by your imagination.  Just think through the whole process before you make any chips.


----------



## JimDawson (Jul 9, 2022)

Here is another one for you to think about.  I'll be making this in the next day or so.

6'' OD x 1'' thick, 6061 aluminum, holes are 5/16 through.  Face, drill, pocket, bore, and profile.

How would you do it?  I'll post pictures of the setup when I get to it.


----------



## Parlo (Jul 9, 2022)

I would tackle this as most have said before if you only want to use a mill.
1. Face both sides to thickness.
2. Drill holes.
3. Drill tapped holes in sacrificial plate + one reference hole in the centre for future use.
4. Screw the blank to the plate and press go.

Check the drawing for the tolerance on the thickness, you may be able to use stock thickness material and skim the faces - only if machining is required on the print. This will give you the edge when quoting as you will save 2 operations and maybe 10% on material cost. It may be worth a quick call to the client to establish the importance of the 1" dimension.

Quick tip. Always drill the parts befiore making the fixture. This way the fixture can be left in position ready for production.

If I had access to a lathe then I would consider starting with tube and facing/chamfering to thickness and roughing out the counterbore within a couple of mm. Then drilling the holes on the mill. And finishing on a fixture as above.

The method chosen all depends on variables such as material cost / time / machine availability / quantity etc...
Larger quantities will lend themselves to multiple fixturing.


----------



## koenbro (Jul 9, 2022)

Do you guys face the stock to final thickness at the start, or do you leave some material (say 20-40 thou) to remove at the very end? I am wondering if the finish gets scratched up during the intermediate steps and is easier to leave some to give it the final surface?


----------



## Parlo (Jul 9, 2022)

koenbro said:


> Do you guys face the stock to final thickness at the start, or do you leave some material (say 20-40 thou) to remove at the very end? I am wondering if the finish gets scratched up during the intermediate steps and is easier to leave some to give it the final surface?


You could rub all the parts on a scothbrite pad when finished machined. I use a scotchbrite disc on a random orbital sander for a satin finish. Either way, any slight scratches will be disguised. So I would machine the thickness first.


----------



## JimDawson (Jul 9, 2022)

koenbro said:


> Do you guys face the stock to final thickness at the start, or do you leave some material (say 20-40 thou) to remove at the very end? I am wondering if the finish gets scratched up during the intermediate steps and is easier to leave some to give it the final surface?


In general, as machined is acceptable.  Most times mill finish and some minor scratching and surface blemishes are acceptable.  We are not trying to make mirrors.  We normally only face from one side for thickness.  The exception to this would be when there is a callout on the print for a surface finish.  Since 99.9% of our work is for our own in-house use, we set the specs on the surface finish.  Most parts are as machined and normal debur.  Some are vibratory finished.  All of our aluminum parts are anodized or powder coated, the stainless parts are as machined.

In the case of the part above, only the face shown needs to be skim cut, just to make it perpendicular to the bore.  The OD and the back do not matter.


----------



## Boswell (Jul 9, 2022)

This sounds like a fun game, I'll play!

1. clamp stock to table on sacrificial spacer (MDF) with clamps that do not interfere with the interior feature. ensure that MDF has roughly corresponding hole in center for step 3 clamping 
2. Mill the interior feature
3. Relocate clamps to inside of part ensuring that they do not interfere with exterior feature. Move clamps one at a time so part does not shift and clamps to not obscure drilled hole locations
4. Mill exterior feature and drill/tap holes


----------



## JimDawson (Jul 9, 2022)

Parlo said:


> I would tackle this as most have said before if you only want to use a mill.
> 1. Face both sides to thickness.
> 2. Drill holes.
> 3. Drill tapped holes in sacrificial plate + one reference hole in the centre for future use.
> 4. Screw the blank to the plate and press go.


Very close to the way I'm doing it.



Parlo said:


> Check the drawing for the tolerance on the thickness, you may be able to use stock thickness material and skim the faces - only if machining is required on the print. This will give you the edge when quoting as you will save 2 operations and maybe 10% on material cost. It may be worth a quick call to the client to establish the importance of the 1" dimension.


In this case this is for in-house use so the 1'' is a ''suggestion''    It will actually be a bit thinner, like about 0.995 or so.


Parlo said:


> Quick tip. Always drill the parts befiore making the fixture. This way the fixture can be left in position ready for production.


We drill parts on the fixture all the time, just be very careful of the drill depth so not to screw up the threads in the fixture.


Parlo said:


> If I had access to a lathe then I would consider starting with tube and facing/chamfering to thickness and roughing out the counterbore within a couple of mm. Then drilling the holes on the mill. And finishing on a fixture as above.


The work could be done on the lathe, but I'm too lazy to stand there and do it. 


Parlo said:


> The method chosen all depends on variables such as material cost / time / machine availability / quantity etc...
> Larger quantities will lend themselves to multiple fixturing.


Absolutely.  Given this is a 1 off, for an in-house project, I have a lot of flexibility.




Boswell said:


> This sounds like a fun game, I'll play!
> 
> 1. clamp stock to table on sacrificial spacer (MDF) with clamps that do not interfere with the interior feature. ensure that MDF has roughly corresponding hole in center for step 3 clamping
> 2. Mill the interior feature
> ...


This is the time to use an aluminum spacer.  I gave your method, using MDF, some thought, and in this case the process can be simplified by bolting down to a scrap aluminum piece.

So here is how I'm doing it.  This is not the only or best way, just how I decided to do it given what I had to work with.

First a quick video of the simulated operation






First the fixture plate.  I found this on the aluminum shelf, was a fixture plate for another project.  Roughly 6x6x0.5



Mount it up in the vice and roughly locate the center hole.  The hole is about 0.377, so a 3/8 dowel pin in the drill chuck makes a good center finder.



Face and drill & tap the 5/6-18 mounting holes.  I can only use 4 of the 6 holes because the existing top & bottom countersunk holes are roughly in line with the part holes.  If four 5/16 cap screws won't hold the part then I'm doing something wrong.



Next locate a fixed point that won't change during machining.  This way if you have a power fail or otherwise lose zero, then you can easily recover.  I used the top, right corner of the vice, and wrote down the DRO position.  Z 0 is the top of the part, so is easy to reset.



X/Y coordinates of the top corner of the vice relative to 0/0.  A vice movable jaw makes a good scratch pad for a Sharpy.



Center up by eyeball, precision is not required at this point, +/- 1/16 or so is close enough.  Plenty of excess material to remove. Clamp to the fixture plate and drill the six 5/16 holes 1.050 deep.  This puts the drill point through the material, but doesn't damage the previously threaded holes in the fixture plate.



Now take a skim cut on the face, about 0.005'', using a pocketing routine.  Now we have a flat surface to work from and that face is complete.  That divot in the lower right (not the one circled in black, the one below it) of the picture is what we commonly call a ^%(&&#* 



Now bolt the part down and remove the clamps, in that order.  Now is ready for the rest of the operations.


----------



## dbb-the-bruce (Jul 10, 2022)

Did you model the bolt heads to avoid collision? I guess as long as your retract heights are above you are probably OK.

I tend to model anything (sometimes roughly - rectangular blob as a clamp for example). Not really needed here as long as pay attention to the linkage moves.

This has been a good thread (I'm still trying to improve my CNC) - Just did a project and used 1/4" dowel pins to align a part that I had to flip over. Worked like a champ.


----------



## JimDawson (Jul 10, 2022)

dbb-the-bruce said:


> Did you model the bolt heads to avoid collision?


No, I just made sure the retract was well above the bolt heads.


----------



## koenbro (Jul 10, 2022)

I very much appreciate the suggestions above and especially the step-by-step by @JimDawson.

I find *fixturing and the second operation* (flipping over, releasing part from material, etc) to be the *hardest part of milling*. I didn't expect this.  I have played for a few years with a CNC router, and usually cut plywood or MDF with occasional 1/8" alu sheet. Always cut through the whole thickness so it is more like 2D milling. I have a sacrificial MDF base with 20mm dogholes and slots, and my fixturing approach is straightforward: push the sheet against dogs and clamp it. Then for the part design 1/4" holes if possible or just hide a few in the design. Drill 5.1 mm holes, tap with 1/4"-20, then use 1-1/2" long nylon screws (McMaster 92929A230) to secure the part. This works very well for the lateral forces seen in routing even with 1/8" Alu. Sometimes with MDF jigs, simple designs, etc I just use pneumatic nails.

For proper 3D milling, I will have to rethink my entire approach. I have a LMS Alu fixture plate that will most likely be the main help. I am not confident MDF can withstand the lateral forces in real metal milling, but I see that that is being discussed by more experienced people, so will keep an open mind.

Here are a few shots of my router setup:

A sheet of MDF from which I cut a circle so my daughter can paint it and wife use is a serving plate. You can see  a few nylon screws that were left in the sacrificial top.



Fixturing sequence (5.1mm - tap - screw), although for this particular case I use pneumatic nails. The screws have slots so they shear off if overtorqued. They are long enough that when using thin material, I can reach below and unscrew by hand, or simply leave and forget.



Big picture:


----------



## JimDawson (Jul 10, 2022)

koenbro said:


> I find *fixturing and the second operation* (flipping over, releasing part from material, etc) to be the *hardest part of milling*. I didn't expect this.


Where possible I prefer to do all of the work from one side and not flip the part over, and I'll go to great lengths to accomplish that.  Including adding screw holes that are only used for the hold down.  But sometimes it is unavoidable.  If flipping the part is required, then dowel pins, or form fit fixturing is the answer.

Here is a odd shaped part that I made for a project, required work on both sides. 1'' thick aluminum.  Note the two drilled holes in line with the T slots, one towards the top, and the other towards the bottom.  There are T nuts staged under those holes



Now I can use those as hold downs



Once the part is completely profiled I need to turn it over and do the work on the other side.



So now we do a mirror and machine a part shaped pocket, about 1/4'' deep, in the MDF.  Note the holes to access the T slots again.



Because the pocket was machined to an exact fit, basically a press fit, I probably could have held it down with a couple of deck screws, which many times I use with MDF.  All of the radial loads are taken by the pocket, you really only need to keep the part from pulling up.  Machining the pocket and the part in one setup insures that everything lines up correctly, both use the same 0/0 setup.






koenbro said:


> I have played for a few years with a CNC router, and usually cut plywood or MDF with occasional 1/8" alu sheet. Always cut through the whole thickness so it is more like 2D milling. I have a sacrificial MDF base with 20mm dogholes and slots, and my fixturing approach is straightforward: push the sheet against dogs and clamp it. Then for the part design 1/4" holes if possible or just hide a few in the design. Drill 5.1 mm holes, tap with 1/4"-20, then use 1-1/2" long nylon screws (McMaster 92929A230) to secure the part. This works very well for the lateral forces seen in routing even with 1/8" Alu. Sometimes with MDF jigs, simple designs, etc I just use pneumatic nails.
> 
> For proper 3D milling, I will have to rethink my entire approach. I have a LMS Alu fixture plate that will most likely be the main help. I am not confident MDF can withstand the lateral forces in real metal milling, but I see that that is being discussed by more experienced people, so will keep an open mind.



I normally just use whatever scraps I have kicking around as fixture plates, be it aluminum or MDF.


----------



## JimDawson (Jul 15, 2022)

Another interesting work holding exercise.  In this case two special T-nuts. This is one of the rare instances that leaving the part attached to the base material makes sense.  I have only actually done this two other times.  In one case it was another set of T-nuts, and the other ''U'' shaped part that did not lend itself to other holding techniques.






So start out with a 1 1/4 x 3/4 x 6 chunk off of the steel scrap excess inventory shelf.  Not sure what it is, A36 or 4140?  Some kind of hot rolled.




Face it off, with a 3/8 end mill, no face mill or flycutter required.  Then cut a dovetail to match the dovetail in the vice jaws.  WAIT! WHAT? Dovetail in the vice jaws?   




Yup, dovetail in the vice jaws.  These are steel soft jaws.  While I own a set of hard jaws, they sit on the shelf and gather dust, I don't use them.  I make steel and aluminum soft jaws as needed, I have even made MDF jaws for special holding needs.  I have been using this particular set of soft jaws for at least 4 years.  Much more versatile than hard jaws, don't kill cutters when you run a tool into to them, as well as being machinable for fixturing as needed.  Make soft jaws, remove your hard jaws, and store them on the shelf.

In this case the shallow dovetail adds an extra layer of security because the part is so tall relative what I'm hanging on to, and I'm taking a 0.500 depth of cut with a 3/8 endmill.  Probably doesn't need it, but only takes a couple of minutes to add the dovetail.  That part is not going to come out of the vise.  I just used a 14° dovetail router bit.



Face off, drill & tap the the holes




About 0.050'' clearance above the vise jaws at closest point.




And done with this side.  Then over to the band saw to trim off the excess.




Flip over and put in the vise




Chew off the 0.181'' excess material.  And done.


----------



## koenbro (Jul 17, 2022)

JimDawson said:


> Another interesting work holding exercise.  In this case two special T-nuts. This is one of the rare instances that leaving the part attached to the base material makes sense.  I have only actually done this two other times.  In one case it was another set of T-nuts, and the other ''U'' shaped part that did not lend itself to other holding techniques.[...]
> So start out with a 1 1/4 x 3/4 x 6 chunk off of the steel scrap excess inventory shelf.  Not sure what it is, A36 or 4140?  Some kind of hot rolled.[...]
> Face it off, with a 3/8 end mill, no face mill or flycutter required.  Then cut a dovetail to match the dovetail in the vice jaws.  WAIT! WHAT? Dovetail in the vice jaws?   [...]
> Yup, dovetail in the vice jaws.  These are steel soft jaws.  While I own a set of hard jaws, they sit on the shelf and gather dust, I don't use them.  I make steel and aluminum soft jaws as needed, I have even made MDF jaws for special holding needs.  I have been using this particular set of soft jaws for at least 4 years.  Much more versatile than hard jaws, don't kill cutters when you run a tool into to them, as well as being machinable for fixturing as needed.  Make soft jaws, remove your hard jaws, and store them on the shelf.
> ...


This step-by-step is very useful, thank you!

I have finished the project from the beginning of this thread. 

I still needed to flip it over. Starting with the blank, I shaped the top, then milled the countersinks, spot- and peck drilled, then milled out the outside contour. Having the TTS system and the sure makes life easy, and a tool touch-off greatly simplifies using one-off drill bits.





After flipping over,  I faced the material to shave off the remainder, down to 5-10 thou. Because the bottom edge had a lip, I had chamfered it 20 thou. This last step required holding in the vice; I probed the middle hole (it is not center, so orientation matters) then chamfer. So it is complicated to design and has three steps. As a hobbyist AND BEGINNER it was acceptable, but I will surely pay attention to streamlining the process from now on.





And here is the final product, assembled: a holder for a Noga mist nozzle to go intot hte recess from the quill lowering assenbly that I removed as a converted to CNC.


----------



## koenbro (Jul 17, 2022)

... and @JimDawson: excellent tip on the soft jaws.  Will do a  pair of Alu jaws and post here the progress.


----------



## JimDawson (Jul 17, 2022)

One thing I noted on your tool path, you are using a lot of step downs.  Normally it's better to use more of the endmill, in other words up to about 3X the cutter diameter step down.  Or in this case full depth on your surface feature, then adjust the stepover from about 10 to 45% of the tool diameter, depending on the material and your machine rigidity.  This gives you much better utilization of your cutter.  In my example above, you'll notice I was cutting 0.500 deep, with a 0.035 stepover, at 8 IPM, 0.0016 chip load in steel using a 3/8 endmill.  That is a very conservative cut, but I was not in a hurry.  At that feed & speed, I think I could have gone 1'' deep with no problems.

The point is that I was not wearing out the bottom 1/8'' of my cutter, I was using a full half inch of it.  I used that same cutter on aluminum the other day slotting at 1'' deep.  It took me a long time to get away from shallow cuts trying to reduce the load, reduce the stepover instead.  This works really well with modern adaptive clearing tool paths, and modern cutter geometry.


----------



## koenbro (Jul 17, 2022)

JimDawson said:


> One thing I noted on your tool path, you are using a lot of step downs.  Normally it's better to use more of the endmill, in other words up to about 3X the cutter diameter step down.  Or in this case full depth on your surface feature, then adjust the stepover from about 10 to 45% of the tool diameter, depending on the material and your machine rigidity.  This gives you much better utilization of your cutter.  In my example above, you'll notice I was cutting 0.500 deep, with a 0.035 stepover, at 8 IPM, 0.0016 chip load in steel using a 3/8 endmill.  That is a very conservative cut, but I was not in a hurry.  At that feed & speed, I think I could have gone 1'' deep with no problems.
> 
> The point is that I was not wearing out the bottom 1/8'' of my cutter, I was using a full half inch of it.  I used that same cutter on aluminum the other day slotting at 1'' deep.  It took me a long time to get away from shallow cuts trying to reduce the load, reduce the stepover instead.  This works really well with modern adaptive clearing tool paths, and modern cutter geometry.


I am happy I posted the toolpath, and am grateful for your comment. Never occurred to me, but I understand what you are saying and will change to use the side of the cutter from now on. Also with these step-downs it took a long time to complete.


----------



## JimDawson (Jul 17, 2022)

koenbro said:


> I am happy I posted the toolpath, and am grateful for your comment. Never occurred to me, but I understand what you are saying and will change to use the side of the cutter from now on. Also with these step-downs it took a long time to complete.


Don't try this at home unless you have enough machine to do it     but it does give you an idea of what modern toolpaths and tooling will do.


----------



## koenbro (Jul 17, 2022)

OK, saving up for a DMG Mori  (but keeping the Precision Matthews  at least for now)


----------



## koenbro (Jul 18, 2022)

I tried to use sidecutting today, and even made the sure in teh setup that the part touches the edge of the balnk, and set the entry point of the cutter there. . I must have done smth worng because I broke the cutter. So I replaced and went back to ramping and multiple shallow cuts.

The cutter has to do essentially a slot, thus two different cuts and that may be the reason for it breaking? Or was I feeding too fast?

1/8" 6061 and a 1/8" 2 flute HSS cutter.
CL 0.001, Spindle 4100 rpm, feedrate 5ipm, 135 SFPM

This is how I fixtured:






After spot drilling, now it's the 5.1 mm (0.201") which is my go to drill as it also allows tapping for 1/4"-20






Broken cutter:





Maybe cut the blank down to almost size and do adaptive clearing from the edge in (instead of 2D contour), so that there is only one direction of cutting?  

It seems that the toolpath strategies are different between 2D cutting (processing a sheet) versus 3D milling.


----------



## JimDawson (Jul 18, 2022)

koenbro said:


> 1/8" 6061 and a 1/8" 2 flute HSS cutter.
> CL 0.001, Spindle 4100 rpm, feedrate 5ipm, 135 SFPM



That gives you a CL of 0.0006 which is fine for 0.125 2 flute cutter.  What was the step over, or optimal engagement?  And more importantly, what did your tool path look like?

Can you post the tool path or a drawing so I can understand what was happening there.


----------



## koenbro (Jul 19, 2022)

Thank you for looking at this @JimDawson .


----------



## JimDawson (Jul 19, 2022)

OK, I see the problem.  You are trying to do a full depth contour into a solid piece.  Not possible without ramping in.   The entire cutting strategy is wrong for that part.  There is no possible way that the tool could straight plunge in and make that cut.  The good news is that it was a cheap tool bit and no real harm done.  

It is possible to make that cut if you use a spiral ramp to depth and then contour, but even that has some major problems with chip clearing since you would be making a full width cut.  And with a small end mill it's really hard to get the chips out of the slot, even with high pressure flood coolant.  So you have to choose a cutting strategy that allows for chip clearing.  Then I'm also trying to figure out how you were planning to hold the part after on the final little bit of cut.

This is all part of the learning experience, and we've all been there.   So lets figure out a better cutting and work holding strategy.

I'm going to make a quick drawing and a tool path for a part that is roughly equivalent to your part, and I'll post it in a little bit.


----------



## JimDawson (Jul 19, 2022)

OK, that took longer than I thought it would

Here is the layout, just a disk with 3 holes in it, but a toolpath equivalent to your part.  The three .25 holes can be used to screw the disk down to something, the outside raw material can be held with clamps.  The circle outside the disk is the outer bounding box to keep it from cutting all of the excess material, which it would do if it's not constrained.


\
And the roughing toolpath



Here are the setup parameters for the adaptive cut.  I chose to use a 1/4'' endmill could have been a 1/8 with some parameter changes.



This video shows the adaptive roughing pass, leaving 0.020 for finishing, and then a spiral down finishing operation for final cleanup.


----------



## koenbro (Jul 20, 2022)

Very grateful for the effort you put in to show the different tabs of the operation (and the video!).  I went through this and recreated the adaptive cutting and simulated it. It is a very different way of thinking about the toolpath than I did before (I think I was still stuck in 2D cutting with a router). Very interesting and I might redo the cut just to see it real life. 

After you leave stock (tab #4 "Stock to leave"), do you go back with an additional operation to clean it up and smooth it?


----------



## JimDawson (Jul 20, 2022)

koenbro said:


> Very grateful for the effort you put in to show the different tabs of the operation (and the video!).  I went through this and recreated the adaptive cutting and simulated it. It is a very different way of thinking about the toolpath than I did before (I think I was still stuck in 2D cutting with a router). Very interesting and I might redo the cut just to see it real life.
> 
> After you leave stock (tab #4 "Stock to leave"), do you go back with an additional operation to clean it up and smooth it?


My pleasure.  I always like to pass on what I learn.  I do have to admit that I was stuck in the same mindset as you, ''this is the way we've always done it'', 50 years of doing it the same way is hard to overcome.  My son finally beat me into submission and changed my thinking. 

Watching this run on your machine or my machine is like watching paint dry, just because of the limitations of the machine.  It looks slow, but it's really removes material faster than multiple step downs, uses more of the endmill, and is more efficient.  When running on the Haas, it no longer looks slow, RPM maxed out at 6000, 80 to 120 IPM feed, frightening to watch.  Because of the shape of the tool path, chip evacuation is greatly facilitated and this is really important, little to no recutting of chips.  One thing you will see when doing adaptive cuts is faceted cuts on arcs, this is normal (it's a roughing operation) and is why you leave stock and make a finishing contour pass.  You can use the same tool for both operations, or use a roughing endmill for the adaptive operation, then come back with a finishing endmill to contour.

If you look at the video again, there are actually 2 operations.  The adaptive roughing operation, followed by a finishing contour helix cut, using the helix ramp function.  I like to do helix finishing cuts where the tool actually cuts a spiral down with a 0.05 to 0.25 step down per pass around the OD of the part.  This is not an actual step down, but is controlled by the ramp angle. It's a continuous cut around the OD (or ID) using all 3 axes in a continuous motion.


----------



## koenbro (Aug 3, 2022)

Hi @JimDawson, I have made several cuts with the method you suggested and I like  it a lot.

With a .25" cutter it is faster, of course, as the chipload I use is 0.001" per tooth. I can appreciate how much material is removed. 

Just to clarify, the second step -- the spiral smoothing is done as a 2D contour, or not? Thank you.


----------



## JimDawson (Aug 4, 2022)

koenbro said:


> Just to clarify, the second step -- the spiral smoothing is done as a 2D contour, or not? Thank you.


Happy to hear that works out for you.

Yes, in most cases I use a 2D contour.


----------



## koenbro (Aug 7, 2022)

Ok I made a cut -- a simple bracket for a control box attachment, and used the sequence you recommended. This short video shows how much material is being removed by a 2-flute .25" mill, and ends with a Tormach SuperFly wreaking havoc:


----------



## JimDawson (Aug 7, 2022)

Looking Good!


----------



## koenbro (Aug 24, 2022)

I have another tool path question. I am trying to machine a simple shape,  2x2" square 6061, 10" long. It will be a hitch recovery (tow) point. The left (far) end will take a steel shackle, the right (front) end will get a rope (soft shackle) so it should have rounded edges to prevent damage to the rope.



What operation should I use for the filleted hole on the right? I was planning to use a HSS ball end mill.

More detail of the top part:


----------



## JimDawson (Aug 24, 2022)

A ball or bull nose endmill would work.  But I might use a corner rounding endmill or router bit if there is enough clearance in the hole.


----------



## koenbro (Aug 24, 2022)

JimDawson said:


> A ball or bull nose endmill would work.  But I might use a corner rounding endmill or router bit if there is enough clearance in the hole.



I am going to take a look at my roundover bits for their radius, etc. What 3D operation do you suggest? As it stands I am configured for adaptive clearing with flat nose mill followed by a 3D contour with a ballend. IS there a better operation? I tried several, some (e.g. "Flow") gave empty toolpaths .


----------



## JimDawson (Aug 24, 2022)

I might try a spiral tool path.  I have used that one before for similar shapes.


----------



## Parlo (Aug 24, 2022)

Plunge a corner rounding cutter into the hole like a countersink.


----------



## koenbro (Aug 24, 2022)

If the radius is right.


----------



## Parlo (Aug 26, 2022)

koenbro said:


> If the radius is right.


obvs lol


----------



## koenbro (Sep 8, 2022)

So here is a one minute video of machining the hitch receiver recovery point.


----------



## koenbro (Sep 8, 2022)

koenbro said:


> So here is a one minute video of machining the hitch receiver recovery point.



Oh, and @JimDawson thank you for the suggestion to use SPIRAL for the filleted hole opening (and for all prior advice). SPIRAL operation with Machine Cusps worked real well using a 1/2" ball end mill.

A project like this doesn't require a thou-level precision for the holes,  but it gave me an excuse to use the Mesa Tool 1/2" x 3" boring bar. 

Quick question: What operation would you use for the flat narrow ends -- I have a Sherline shoulder fly cutter and tried to use FACE but did not work. I ended up using a regular 1/4" endmill but it left grooves. Although for this project it doesn't matter, would like to know for the future.


----------



## JimDawson (Sep 8, 2022)

koenbro said:


> Quick question: What operation would you use for the flat narrow ends -- I have a Sherline shoulder fly cutter and tried to use FACE but did not work. I ended up using a regular 1/4" endmill but it left grooves. Although for this project it doesn't matter, would like to know for the future.



Do you mean where the shackel attaches?  I would most likely use a 3/8 endmill to rough that out, then go back in with a 1/2 ball to finish.  If you're not in a hurry, use the 1/2 ball and do it all in one pass with a 0.005 stepover.

I don't understand why you were left with a rough finish, you would be able to see marks, but should not be able to even feel them when done.  Dull endmill maybe?  Slightly out of tram?  I'll draw that up and try a couple of different cutting strategies, and post them.


----------



## koenbro (Sep 8, 2022)

The surface is smooth just has the visual pattern, whereas the flycutter would leave mirror-like. Just want to improve my skill set for the future.


----------



## JimDawson (Sep 9, 2022)

koenbro said:


> The surface is smooth just has the visual pattern, whereas the flycutter would leave mirror-like. Just want to improve my skill set for the future.



Ahh, well then I would rough it out, finish the fillet with a ball end, then a final cut across the face with the fly cutter.  That would give you the tool mark pattern you want.

The other option is to flip it up on the side and cut it with the side of the endmill.


----------



## Parlo (Sep 9, 2022)

koenbro said:


> The surface is smooth just has the visual pattern, whereas the flycutter would leave mirror-like. Just want to improve my skill set for the future.


Use scotchbrite on a random orbital sander, choose the abrasive grade to suit the level of finish required. It is extremely quick and gives nice finish options from satin to mirror.


----------



## koenbro (Sep 9, 2022)

JimDawson said:


> Ahh, well then I would rough it out, finish the fillet with a ball end, then a final cut across the face with the fly cutter.  That would give you the tool mark pattern you want.
> 
> The other option is to flip it up on the side and cut it with the side of the endmill.



The final cut with the fly cutter would be a FACE operation? I need to select a surface and then oddly, the flycutter overshoots that, meqnaing it goes in farther. I am going to try that again and post the screen grabs. 

Flipping it on its side sounds great actually!



Parlo said:


> Use scotchbrite on a random orbital sander, choose the abrasive grade to suit the level of finish required. It is extremely quick and gives nice finish options from satin to mirror.



Yeah I will have to try that.


----------



## JimDawson (Sep 9, 2022)

koenbro said:


> The final cut with the fly cutter would be a FACE operation? I need to select a surface and then oddly, the flycutter overshoots that, meqnaing it goes in farther. I am going to try that again and post the screen grabs.


I think the TRACE function would work for this, or just a manual jog across the face.






koenbro said:


> Flipping it on its side sounds great actually!


----------



## koenbro (Sep 9, 2022)

Seems more complicated than I thought . TRACE is shown here:



ADAPTIVE overshoots it as does FACE:


----------



## JimDawson (Sep 9, 2022)

The TRACE tool path runs the tool center line right down the trace line, much like ENGRAVE.  That's the reason I drew the sketch line where I did, and assumed a 2.25'' dia cutter.  This should put the edge of the tool right at the front edge of the fillet.  Sometimes you have to make some changes to the drawing to get it to cut what you want, then revert back to the original drawing for other features.  I use TRACE when there is no there reasonable way to do it.

You can also use a 3D adaptive and constrain the cut area with a sketched box.  You can always make it do what you want, but sometimes requires a bit of fiddling. 

Here is an example of a 3D adaptive roughing cut


----------



## JimDawson (Sep 12, 2022)

Here is a real world TRACE tool path.  I made a measuring error on the flywheel for my tube polisher project and of course transferred that measurement to the drawing without double checking.  No real problem, but I need another 1/8'' clearance in the pinion gear housings.

I need about 1/8 more clearance here.



The left side is what I have now, the right side is what I need



There are several ways to do this, but I chose the simple method and will be cutting some air.  I could have constrained the adaptive clearing with a bounding box to reduce the air cutting, but I'm not in that big of a hurry and air chips are easy to clean up.  



Then I decided to make a final 0.020 contour pass to finish cleaning up.  I could have just set the adaptive clearing to leave 0 stock and not even done a finishing pass, but what fun is that.  But when I tried to do a 2D contour it insisted on taking a cut all the way around the part rather than just the face I wanted to cut.  I could have constrained a 3D contour with a sketched bounding box, but I insisted on making it do what I wanted with a 2D cut.

This is where TRACE comes in.  First I drew a 13.5 dia circle, then offset the the circle the radius of the 3/8'' endmill (0.188) from the surface I want to machine because the tool center line follows the trace line.  Then drew the two cut lines where I wanted the endmill to start and end, then trimmed away the rest of that circle.  So now I have a tool path to follow exactly where I want to cut.




So now all that is required is to go into CAM, select Trace and select the line.  Since the line is at the top of the part, I also needed to set the axial stock to leave at -0.645 to reach the bottom of the area I want to cut because the trace function cuts exactly on the line unless you tell it otherwise.  You also can use multiple step downs if desired.




Now I just need to go make some chips.


----------

