2D High Speed Toolpath, Blend Mill?

[Donkey Hotey]

I've got a problem in X4 MU2 and I'm not sure if it's something I'm doing wrong or if it's the software.

I have a wide slot I need to clear (about a foot wide). I'm currently using Peel Mill. The problem is that it only cuts in one direction and all the rapid-return motion seems to add unneeded time to the cycles. Zig-zag would be preferable but, it doesn't offer that.

Blend Mill is another one of the options in the 2D HS milling. It looks like a similar toolpath but, DOES offer a zig-zag option. The problem is that when I try to regenerate the toolpath, it says,

"Blend mill does not (yet) compensate blend chains for tool."

After that, it posts some weird toolpath, off the part in space and rotated away from everything else. What does that mean? Does it mean, this doesn't work in this service pack, go away? Or am I giving it bogus geometry?

The geometry is a straight line down one side and a spline contour on the opposite wall. The slot is open at the start and finish. Anybody?

[Superman]

Why not use "Pocket" ?
it offers the use of "Open pockets" , and probably faster clearing strategies

[Donkey Hotey]

I'm all ears (edit: that's kinda' funny when I see it posted next to my avatar ). This is being done on a Haas GR712 (gantry router). It's not a very powerful spindle and it doesn't like heavy side loads. The machine screams if I can keep a 3/4 4-flute at about 5% stepover. Any more (or less) and it vibrates and chatters like hell. Here are the other methods I tried:

None of the pocket methods seemed to offer anything better to clear the material. Constant Overlap Spiral is probably the best one for this machine but, it involves lots of wasted time recutting the same edges over and over. The slot is about 1 foot wide and 3 feet long. The spiral ends wayyy too soon on the two walls, then spends a lot of time running over the boundaries over and over.

The constant overlap options, including 'clean corners' all overwhelmed the spindle and the cutter when the engagement went up in the corners (remember, I'm trying to keep lateral engagement to around 5% or 0.035"). High Speed pocket took 9 freakin' hours to clear two of the pockets I described. It spent more time in the back-loops than it did engaged in the cut. If that one had a zig-zag option, it might have been better.

Blend mill is clearing the two pockets in about an hour and leaving an acceptable finish. I was trying to improve that (this is just part of the cutter path and I have to make 4 more of these parts).

So did I miss something? Blend Mill really looked promising. All I wanted to do was keep the cutter in constant engagement. I'm trying to learn some of the new features in X4 and I'm not sure why Blend Mill wouldn't work in this case.

[Superman]

Greg
Can you give a little more info about the machine and the material being cut ? aeropart?
how high are the walls ?

gantry-OK, what holders ? ( BT50 etc ) , max RPM ? , how it corners with higher feedrate ? coolant /air supply ? etc
What's it like for grunt with low RPM ?

If steel or going into the exotic materials, I'm leaning to using a feedmill to get material out
Say a 2" OD like this would be nice -
S600, DOC 0.025 to 0.035"", Feed/tooth=0.04" , climb cut, 60% stepover
But you could come down to a 1" cutter---DOC has to be less than the Ap, feed is still high, about 0.04" per tooth
cut speed for Ti about 45 M/min, steel -100 to 150 M/min, Al-300 to 500 M/min ( I'll let you convert )

If alum. or softer, I'd try a larger cutter with a decent corner rad to get material out
HSS or Al grade CBD cutters - to work similar to the feedmill but slower feeds and larger DOC

The tip having an approach angle tends to allow the cut forces to travel up the spindle axis instead of being 90° to it, the higher feedrates don't really allow the machine to chatter---it is adviseable to make the toolpath place arcs in corners ie pocketing - high speed,
you can 2D contour, but modify the profile geometry to have arcs larger than the tool radius.
Shredmills work good on steel & Al, but tend to throw the Al chips everywhere, they tend to jamb up the toolchangers on our Okumas
Plenty of coolant to stop re-cutting of chips, also stops the cutting edges being damaged

Being a gantry, I'd say guarding is minimal, so you may have a nice mess on the floor, maybe air mixed with minimal coolant ?

Cutters should be as close to the spindle nose for best performance

Steve

[Donkey Hotey]

Ahhhh....Steve...I see that you're not familiar with the Haas Gantry ROUTERS. It's not a MILL. It's basically the CAT40 spindle from their Toolroom mill. I think it's rated at 15 HP but half that is more likely. It's 10K RPM, with no gearbox. This particular machine has the extended Z travel option so when it's down at the table (like this case), the spindle is extended all the way out and it's springy as hell. It's one of these but with riser blocks on each side that raise the bridge and add 18 more inches of Z travel:


With that said, we're learning that if we get the parameters right, it will remove an impressive amount of material and still maintain a good finish and hold a reasonable tolerance for what it is.

Two weeks ago, we had the same 4-flute, 3/4 endmill, buried an inch deep in 6061, 5% engagement, .010 (calculated) chip load, 10K RPM and 480 IPM. It was clearing so much material that I had to pause it every minute or so, just to shovel the chips away.

Through testing, we found that any less than 5% puts too much side load on the cutter; the tooth simply doesn't approach the wall at enough angle to actually engage cleanly. It chatters and screeches and acts like it's overloaded.

Much more than 5% does the same thing but, now it's in the feed direction. The machine just isn't rigid enough to handle really pushing a 3/4 endmill into a wall of material. At that magic 5%, we can push the machine as hard as we want speed-wise and it just sings. We haven't tried a six or eight flute yet but, we have no reason to think it won't work just as well. We were at a steady 60% spindle load (spiral pocket) and the chips were perfectly formed.

Interestingly, we found that the 5% caries over to other sizes which is why I think it's about the cutter angle approaching the work rather than the actual amount of material being engaged. A 1/2" endmill doesn't like the same engagement amount as the 3/4 (0.035") but it does like 5% (0.025). This is why the method I use for clearing the material is so critical. Anything that changes the engagement angle abruptly just doesn't work with this machine.

Peel Mill really works great but, it's wasting all the back motion time when it could be cutting. We're not actually finishing a wall with this operation so climb/conventional makes no difference.

This particular part isn't very deep. I'm only clearing 0.125" deep of material. It's actually facing these two, wide swaths, down either side of a mostly flat plate. I needed a cutter path that I could contain between the feature in the center and the rows of clamps on the left & right side of the part.

I really would like to know why I get that error with Blend Mill, even if it's not the right cutter path for this application. I may need it in the future and it doesn't seem to be working. Of course, I'm also open to other suggestions. I'm also trying to learn all the pros & cons of each cutter path so I can effectively use them. Every new part is a chance to experiment.

[tony978]

I would say if your not looking for a high finsh a dura mill rogher would work better ( from Series ACR-3) . That should help with being able to get away with a greater step over .

Tony

[TheBigJW]

From another site.

http://www.shopwareinc.com/downloads...hstwebinar.wmv


John

[Donkey Hotey]

Originally Posted by TheBigJW From another site.

Wow, John, thank you. That was a PERFECT video for what I was looking for. I've watched the first 50 minutes and I'm at saturation. I'll watch the rest tomorrow.

At least I now know what the error I was getting means. Now it seems that it's actually generating a bogus toolpath and that error had nothing to do with it. Blend mill is generating a toolpath wayyy outside the boundaries of the part. It's a disaster. I thought it was some kind of error detection that ensured you couldn't run the toolpath if it mistakenly posted a bad path (well outside the machine boundaries).

I'll see what I can do with it tomorrow with what I've learned from that video. Thanks again.

[VWbmx]

I assume when using Peel Mill you are increasing the back feed to the machines maximum allowable feedrate and only microlifting .003" max.
I've never had to machine such a big slot but Peel Mill seems to kick a$$ at material removal.
Keep us updated because I've had that same spiraling out of control toolpath using Blend Mill also.

[Donkey Hotey]

Yes, I was using the max feedrate but, it still seemed to spend a lot of time in the air. I actually took out the microlift because it seemed to pause slightly at the lift & drop points.

I've attached the file to this post if any of the X4 gurus want to take a look. It's building the Blend Mill toolpath out in space. I have no clue why. If I change it to Peel Mill, it puts it in the right place. This is the original error I was having and I thought the message had something to do with it.