Machsupport Forum

General CNC Chat => Show"N"Tell ( What you have made with your CNC machine.) => Topic started by: BarryB on January 24, 2010, 07:55:28 PM

Title: rough cut prob
Post by: BarryB on January 24, 2010, 07:55:28 PM
hey folks, I've finally got my issues with the smoothstepper and mach in order and am now doing a big rough cut.  I'm running into an issue where the bit is starting to bite into the wood instead of smoothly cutting.  I little roughness is fine, since this is a rough cut, but it was really biting.  I caught it a bit too late as the bit broke;(

(http://www.3dmation.com/images/ru_cnc/prob.jpg)

This is happening about 3/4 the way through the rough cut.  The beginning was fine.  The depth I'm doing is 9mm, so not too bad and 90mm/min feed, nothing crazy.  The bit is double fluted 6.35 mm, downward spiral.  My overlap is 5mm for the roughing.  The spindle is spinning, approx 14,000 rpm.  Is this an indication of the bit wearing out?  Or should my feed rate be slow, or should the spindle be spinning faster?  Maybe the depth is too large?  Is my overlap too large?  Should I use upward spiral instead?  I don't think the feed rate is too slow, as it's almost intolerably slow;)  I was thinking of increasing the feed rate till I saw this happening.  I'm new to this, so this like most issues is an all new problem to me.  So you people that are more used to issues, please let me know what you think.

Barry
Title: Re: rough cut prob
Post by: ger21 on January 24, 2010, 08:21:01 PM
Try 3000mm/min, or even faster at 14,000 rpm. An upcut might be better, but is more prone to tearout. YOU should be OK with 9mm depth, but you might want to try 5-6mm and see if it's better.

However, it appears that you have some serious flex in your machine. Or something is loose. I honestly can't see the cut being that rough without the whole spindle shaking that much.
Title: Re: rough cut prob
Post by: ostie01 on January 25, 2010, 02:17:29 AM
Hi, I agree with Ger21, look like there's a lot of vibration along your cut, you could post some pics of your setup.

If the bit produce loud noise when cutting, reduce cutting depth , will help.

Jeff
Title: Re: rough cut prob
Post by: BarryB on January 25, 2010, 10:20:54 AM
The only flex I have in the machine is from the B/C drive itself.  The rest is really really sturdy.  I'll try using an upward spiral, and a shallower depth.  I think the 5mm, stepover might be a bit much too.  I'll make it the radius of the bit instead.  I did notice one thing after looking at the bit.  The plastic clamps I was using were cut into with the bit and I think it acted like glue to the bit.  I think that's one of the reasons the bit was biting.  Hopefully I'll have more to show very soon.

Barry
Title: Re: rough cut prob
Post by: ger21 on January 25, 2010, 06:36:32 PM
5mm stepover should be no problem at all. I've heard of people using 1/4" bits cutting 10mm deep, at 15,000mm/min.
Are you sure the part isn't moving? The only reason the bit would be grabbing is if there's play in the system somewhere. Either in the machine, or in the part.
Title: Re: rough cut prob
Post by: BarryB on January 25, 2010, 06:41:20 PM
As I stated before, that only play I see right now is from the B/C head itself.  I suppose that could cause the issues, but that's not something in my control to fix as it's 3rd party.  I have to investigate the other avenues first.

15000 mm/min, that's just crazy to me.  He must have a very high hp machine, mines only 2 hp on a gantry with the b/c head.  There's no way I could move mine that fast.

Barry
Title: Re: rough cut prob
Post by: ostie01 on January 25, 2010, 08:08:57 PM
5mm step over with a 6mm tool is almost full cutter, prone to vibration, would try step over less than half the bit, like 3mm and you could increase feed.

Jeff
Title: Re: rough cut prob
Post by: ger21 on January 25, 2010, 10:51:16 PM
I've been routing wood with a $150K cnc for over 10 years. The stepover is not the problem here. You can cut wood all day with a 100% stepover with no problems.

My homebuilt mdf and plywood machine has a fair bit of visible flex, and the worst cut's I've seen from it are infinitely better than those.
Title: Re: rough cut prob
Post by: BarryB on January 26, 2010, 12:18:03 AM
No need to get testy.  I think by your own definition this is probably not flex since your plywood/mdf machine has a fair bit of visible flex.  This is a extruded aluminum and aluminum plate router.  The flex is nearly nonexistent.  I could probably stand on the gantry if I wanted it and it wouldn't flex visibly.  The only flex, I can discern is from the B/C head and even then it's so incredibly small.  I'd have to pull on it, with I bet about 70 lbs force.

I took the part and jig pieces off the table.  Remember I said the bit went through the plastic jig and basically melted it?  Well, I'm willing to be that's the reason the bit was biting.  Look at this:

(http://www.3dmation.com/images/ru_cnc/prob2.jpg)

(http://www.3dmation.com/images/ru_cnc/prob3.jpg)

I bet that melted plastic basically acted like glue and the bit never recovered from it.

And, btw, these jigs aren't really meant to secure a part to a table.  I need to make some that do.  They were the closest thing I could find at the hardware store;)

Still though, I'm going to try out everybody's suggestions.  For the next test, I'm going to use a 3mm stepover, 5mm depth, 160mm feed rate, upturn bit, and 14,000 rpm.  Wish me luck.

Barry
Title: Re: rough cut prob
Post by: mhasting2004 on January 26, 2010, 02:07:03 AM
Hi Barry

Just an observation... the first pic shows several steps in the work piece with 2 board thicnesses above the bottom piece. However there are similar gouges in each layer (different z) and this seems to indicate the tool path was similar in each... Highly unliely that this was vibration as they were cut at different times if I'm seeing right. Can I make the suggestion to rerun the code at a much slower rate to air cut over what you have already done and see if it follows the same path.

You're not using some high speed machining paths are you? Whats the gcode look like? is it using circular interpolation of short vectors?

Might be way off but maybe food for thought.

Cheers
Title: Re: rough cut prob
Post by: BarryB on January 26, 2010, 10:33:45 AM
Thanks, I'll check.  I've no idea if this is set for speed machining.  I'm currently doing this with MeshCAM, as I'm still deciding on a 5 axis CAM software.  In MeshCAM there is a quality level, which is currently at 2.  I'll increase that for the next cut too, which I'm hoping will be tonight.

Barry
Title: Re: rough cut prob
Post by: ger21 on January 26, 2010, 04:50:29 PM
Quote
I'm currently doing this with MeshCAM

That's some critical information. Not sure what you're part looks like, but it appears to me that MeshCAM is the wrong tool for that type of part. A 2D CAM program could give you much more efficient toolpaths, that would probably reduce machining time by up to 75%, maybe more. With MeshCAM, more than likely, you probably ended up with a lot of plunging, which is bad with your downcut spiral. And the rough cuts that I thought were play in the machine, were probably due to MeshCAM's roughing toolpaths.

You didn't show a picture of the bit, but did it have a lot of plastic on it? It's pretty hard to break a 1/4" bit in wood, unless you get it pretty hot. But normally you'd see a lot of burning, and I don't see it. So if there was plastic on the tool, then there's a good chance that's the reason it broke.

I've been a MeshCAM user since the very first beta, and am also a moderator on the MeshCAM form, so I have plenty of experience with it.

Can you show a pic of your part? Were you going to use a ballnose bit for your finishing passes?
Title: Re: rough cut prob
Post by: ger21 on January 26, 2010, 04:54:24 PM
Oh, almost forgot. I wasn't being testy. :) Just trying to point out that I know what I'm talking about, and was disagreeing with the previous poster. And a few others. With wood, the general rule is to cut as fast as you can, provided you get acceptable cut quality. Disregard the quality of this particular part for now. Stepover is not really important when roughing wood, as you can easily use the full tool width. And if the chip load is not kept up near the recommendation, your tooling life will suffer.
Title: Re: rough cut prob
Post by: BarryB on January 26, 2010, 05:05:16 PM
Hi, yup, the bit was blackened and had bits of plastic still on it.  I didn't save the bit, threw it away last night.  There is a spot where the bit plunged into the wood just after melting the plastic.  There is plenty of burning there.  That's in the pict.  I'm trying to save the part as a surprise, so can't show it just yet.  I think people will really like it;)

That's good to know about you being the moderator for MeshCam.  I'll hit you up for tips I'm sure.  I may be switching to RhinoCam in the future though.  The machine is 5 axis, and I use Rhino to model with.

Ballnose bit?  You mean there are other styles?  I hadn't bought a ballnose yet, only flat ones.  I do have a 1/8 inch flat though.  Perhaps I should get a 1/8 inch ballnose for the finishing;)

Chip load?  what does that mean?

Barry
Title: Re: rough cut prob
Post by: ger21 on January 26, 2010, 05:19:11 PM
https://www.onsrud.com/xdoc/FeedSpeeds
Title: Re: rough cut prob
Post by: mhasting2004 on January 26, 2010, 05:23:06 PM
Hi Barry

My CNC is not running yet but here's a good site I found to calculate chip loads and cutting speeds in various  materials:

https://www.onsrud.com/xdoc/FeedSpeeds

Chip load is basically how hard you are pushing your cutter, it includes feed rate, step over, depth of cut and material hardness.

Cheers

Mark
Title: Re: rough cut prob
Post by: mhasting2004 on January 26, 2010, 05:24:05 PM
Your too fast Ger :)

Title: Re: rough cut prob
Post by: BobWarfield on January 27, 2010, 11:18:00 AM
Hi, yup, the bit was blackened and had bits of plastic still on it.  I didn't save the bit, threw it away last night. 

You wanna kind of throw out those important clues up front to help the helpers!

LOL, I primarily stick to metal, but have to admit that was looking pretty gnawed.  Had to be something seriously off, and Gerry and the others were trying to get at it.  You want to keep a close eye on your cutters any time you have a little problem.  Should be nothing sticking to them and no discoloration.

Speaking of Onsrud, I'm getting ready to add wood to my G-Wizard feeds and speeds calculator.  Their feeds and speeds data is by far the best I've found so far.  Wood is basically pretty hard to track down.  Do you fellas have any other good sources of that data?

Cheers,

BW

Title: Re: rough cut prob
Post by: BarryB on January 27, 2010, 12:03:09 PM
Btw, I used the settings I mentioned above as a new test.  This finished no problems, and the cut is really sharp across the board.  I did put in the wrong bit profile for the finishing stage, but only mismeasured the length of the flute.  This made it burn in a couple spots, but otherwise, looking good.  Onward and upward.  Thanks for the info.  When this part finishes, I'll post picts in a new thread.

Barry
Title: Re: rough cut prob
Post by: robgrz on February 17, 2010, 01:11:09 AM
Barry-

I would also download the latest V3 beta of MeshCAM from http://www.grzsoftware.com/v2dl.php .  It has a totally new roughing system that is likely to give a much more accurate and smooth toolpath, and you'll never have to worry about "quality" values for roughing again.  Even though it's marked as a beta it's fine for day-to-day use.

-Robert
Title: Re: rough cut prob
Post by: BarryB on February 17, 2010, 02:29:22 PM
Thanks, I've decided to go the RhinoCAM route.  One because I use Rhino, but another is that the machine is 6 axis, and Rhino CAM will work with 6 axis indexed.

I should stress though, the rough cut problem I was having was NOT due to MeshCAM, it was mainly due to the part not being held down stiffly enough and clamping in a way that my bit wouldn't eat into its supports.  MeshCAM works fairly well.  There are a few issues, like pocketing.  I didn't like how it did that, and it had a lot of unnecessary plunges, but other than that, it's well worth the cash.

Barry
Title: Re: rough cut prob
Post by: jonny quest on February 18, 2010, 04:32:49 PM
Look into Madcam. It's Rhino based and supposedly very good.

I'm going the Madcam route in a few months.
Title: Re: rough cut prob
Post by: Chris.Botha on February 18, 2010, 06:20:49 PM
RhinoCam gets my vote :) i do unusually complex cutting and find that RhinoCam always gets me there.. its ass slow on rotary code generation tho....
Title: Re: rough cut prob
Post by: BarryB on February 18, 2010, 06:23:53 PM
I met with the RhinoCAM folks, and believe they have my business.  It helps that I work just down the street from them too.  If I find an issue, I can just zip on over and bang some heads;)

Barry