Bumps on profile cuts

I am using a 1/2" diameter, 2.5" cutting length straight bit to cut a guitar body with lots of 2D curves on 2" deep profiles (in four passes.) For now, I'm using MDF for prototyping. I need to eliminate the need to shape the part after cutting so the customer really just needs to sand down the roughness of the grain. However, whenever I cut the part, I get very noticeable bumps. I've correlated these to several factors:

1. I consistently get a bump where the circular lead ins meet the cutting line
2. There are bumps on either end of a zig-zag ramp lead in
3. Where the part gets close enough to the edge of the material that the bit cuts through the edge, there's a noticeable bump.
4. I think I can even attribute one bump to a ramped tab.

I think I can probably eliminate most of this by using spiral ramps and steering clear of the material edge. I won't be able to do away with tabs, but I'm not 100% sure about the tabs causing the bumps anyway.

I'm wondering though, should the spindle have that much play that a bit will move by ~1/16" based on what I would consider normal cutting forces?

Are there other factors at play that I can tweak to improve the smoothness of the cuts?

Thanks a lot!
Andy

This sounds like a deflection issue. Which direction are you cutting? Climb? Conventional? I would try climb milling with a .0625 offset and leaving an onion skin on the bottom of the part and popping a starter hole all the way through for a flush trim bit to release it. Since it'll be ash you're milling, i would mill across the end grain at the neck and any other sharp corners in the design. Same technique you would use if using a hand router on the edges of a board. Across the end grain first then the sides. This helps avoid chips and tearout. Once that's done i would repeat the process at full depth of cut in conventional. If you use a lead in of .0625 to the final profile taking off that excess left behind, the bit wouldn't need a ramp plunge. It would simple plunge where the material has already been milled. The big difference here is where that bit deflects. When cutting in the climb direction (clockwise around the part). The bit would normally deflect away from it. With conventional dirrection (counter clockwise). It deflects into the part. Considering that you'll only be taking off 1/16" of material, the deflection on the final pass would be minimal.

Regards
Randy

Thanks, Randy! I'm reading into your post that the flaws should be expected and are normal with the approach I used.

I was cutting "conventional" (counterclockwise on outside cuts.)

I'll give the "sneak up on it" and onion skin approach a shot.

Do you think I should still cut the .0625" final cut in passes? It seems to me that it'd be cleaner just to cut the full 2" depth in one shot.

Thanks a lot for sharing your expertise!

Andy

Probably easily missed but yes, final cut down to full dept minus the onion skin. You shouldn't have to step that cut.

When you run for first stepped cut, pause for a min and take a look to see if there is any deflection into the material at all. If there isn't you can cut the offset to less then a 1/16th or if brave, no offset at all. If the issues continue then there may be other things you'll have to look at.

Regards
Randy

Andy; I will often cut hardwood as outlined by Randy's excellent advise. I usually program the conventional cut in one pass on the same vector as the climb cuts with hardwood. Easier to program, and the the conventional cut just cleans up the material left from the climb cut bit deflection. Also make sure to extend your final cut well past the start point and ramp out. (up to .5")
Bob

Randy, Bob -

Wow... It's amazing what you miss when you read things too quickly and before the coffee's had a chance to kick in. Like, the whole point of the post. :eek:

Thanks for the great tip! I'll give it a shot.

Andy

Some deflection is normal but 1/16" is rather a lot. With the spindle OFF grab the collet and wiggle it back and forth. If you can feel any play there is slop in the machine that you might be able to minimize by checking all bolts, wheels, etc for proper tightness.

David - I suppose the fact that I hadn't yet checked for looseness in the assembly makes it appropriate that you warned me to turn the spindle off before grabbing the collet. ;) I'm not going to have a chance to actually try to cut a part again for a while, but I will check the spindle right now. I'm going to kick myself if that was the problem!

Thanks for that!
Andy

The spindle assembly is rock solid. There is no wiggle in the z or y direction. However, with a bit of oomph, the x axis does move a little (~1/16"). My guess is I need to make sure the gear on the stepper motors are mounted as snug to the rail as possible since the motors themselves are on tight. That's the only adjustment I can think of.

I don't think this is the only cause since I'd only see bumps in the x direction if it were. I'll try the climb/conventional cut combo in addition to tightening the stepper motors.

Andy

Just be careful not to make them too tight. I've heard from the PRS guys not do over do it. I've got an old PRT

By the way, what brand bit are you using? I've used the same style and size bit before and had the exact same thing happen. It was a cheaper bosch bit.

It's a Bosch bit, wouldn't you know it.

What do you use instead?

Andy, I would definately recommend getting bits that are designed for CNC. if your tolerence is tight. They have slightly different geometry than plain old router bits for general woodworking. There are plenty of brands out there (different people swear by different companies) Centurion, Amana, Onsrud are ones I've had good luck with.

Always worth checking the simple stuff first. Also check that the pinion gear is on the shaft tight if you have play in only one axis.

Thank you all for your input! I'll post when I get a chance to implement all of these tips and get some results.

Andy

Quote:

---

Originally Posted by asteude

It's a Bosch bit, wouldn't you know it.

What do you use instead?

---

I don't usually do to much more then a typical 1/4 or 3/8 dia spiral bit will handle so i actually usually just run to lowes and pick up the very same bit. Let the other guys that run into this more often give you recommendations. Onsrud is always a good choice however.

Quote:

---

Originally Posted by shoeshine

Andy, I would definately recommend getting bits that are designed for CNC. if your tolerence is tight. They have slightly different geometry than plain old router bits for general woodworking. There are plenty of brands out there (different people swear by different companies) Centurion, Amana, Onsrud are ones I've had good luck with.

---

I found a Whiteside bit that'll work. The part #'s for their CNC bits appear to start with "C" and are otherwise the same as the handheld router bits. So, the bit I ordered, C1072, is the CNC equivalent of the regular 1/2" diameter, 2" cutting length, 1/2" shaft bit with part #1072. I found the best price on www.carbideprocessors.com.

Hartville tool gas a Whiteside 1072 for $22.19 with free shipping. I am not sure if you can join the router bit club that after you purchase so many bits you get to choose a free one. I belong but I go to the store and pick them up.

Quote:

---

Originally Posted by jerry_stanek

Hartville tool gas a Whiteside 1072 for $22.19 with free shipping. I am not sure if you can join the router bit club that after you purchase so many bits you get to choose a free one. I belong but I go to the store and pick them up.

---

That's a great price for that bit! I don't see the CNC version on their site though (C1072.)

I made the following changes:

1. Climb cut first followed by conventional cut
2. used onion skin instead of tabs
3. got rid of leads and used spiral plunge instead
4. used a specialized CNC bit (Whiteside C1072)

I didn't tighten the step motors yet. I may still do that if I run into problems down the road. For now, I'm a little worried about overtightening them.

The first cut I tried was perfect... until the part broke loose because the material thickness was off and I cut all the way through the material. I'm now changing the "onion skin" to, perhaps, an "elephant skin" to be able to absorb a little variance in material thickness.

Thanks for your help, everybody!!

Andy

Quote:

---

Originally Posted by asteude

I didn't tighten the step motors yet. I may still do that if I run into problems down the road. For now, I'm a little worried about overtightening them.

The first cut I tried was perfect... until the part broke loose because the material thickness was off and I cut all the way through the material.

---

If you are running a PRS - it is impossible to overtighten them. On a PRT the correct tension is 3.5 turns on the buckle just as the spring starts to get some tension on it.

Also, flatness of your spoilboard is paramount. It will haunt you forever and mess up jobs etc if it is not glued down to the plywood support board - with zero screws in the lamination. It should be machined flat with a large diameter bit so that table is true to the tool. This will remedy the 'cutting deeper here and shallow over there' condition. - Provided that the parts are being held down correctly.

Flatness is very important. A few cutter kerf tracks here & there isn't.

-B

Brady - could you explain why you say you can't overtighten the motors on the PRS? I imagine you could cause undue stresses and wear on the motors if the gears are engaged too tightly.

My spoilboard is in dire need of being replaced, but it is glued and flat where it's not shredded by innumerable screw ups.:D

Andy

Brady: there is a good point there. You can put quite a bit of pressure from the motors pinions to the rack on a PRS and have no problem but I wouldn't suggest doing something like pulling them up with a clamp tightened heavily as the engagement could then be so tight that you would blow a driver trying to move.