[johnno402002]

Hi,
I'm working on the first part on my new SVM2, and I need some help with speed and feed settings. I've broken three cutters so far, one before it took a cut, I dropped it out of the spindle straight on to the vice jaw, the second I machined the vice jaw ( video at silentworkshop.com), and now the third by what I think is having the wrong feedrate. My vice now has rigidity problems, it's quivering wondering what I'm going to do to it next....

The attached picture shows the last cut, it's in mild steel, 4mm dia coated carbide ball nose mill, cut width 4mm, depth 2mm, spindle at 6000 rpm ( max spindle speed) feed at 150 mm/min, under flood coolant. It seemed to be cutting fine until it broke, the surface finish in the cut is good, looks much better than it shows up in the picture. I checked the cutter temp as soon as the machine stopped, it was cold, it's cutting edges are still perfect. It had broken off up at the collet. I think I know why, I calculated the feed rate from the cutter manufacturers data, but I missed that is was based on 0.25 D side cut. I also checked it with Bob Warfield's gwizard, and it gave very similar settings, except it showed the cutter deflection in red, which I also missed . So I think the feed rate was too aggressive. Looking at it now, I can also see that it wandered off at the start of the cut, I could not see that when it was cutting under the coolant.

The part itself is an exercise to set a style for all the brackets in a 1930 Ford Tudor hot rod I'm setting up to build, I'm trying to get something that is practically machinable but rather different to anything you can buy off the shelf. I still have a long way to go to work out how to best size it's features, the order of cutting operations, how to hold it, just about everything really. I now know a few things not to do.

I do have some cnc experience, but it was a long time ago, we were simulating the cutter paths on an Apple 2 E and a Roland plotter if I recall correctly.

Given that I have no experience in setting the speeds and feeds correctly, any advice on how to make this would be greatly appreciated.

regards,

John

[johnno402002]

Picture of the partAttachment 313990

[Tkamsker]

i would try less deep like 1 mm 120 feedrate the rpm is ok but it is jzst a 4 mm miller do the machine vibrate ? if yes you try 0.5 mm deep cut i would rough as much as pissible and only cut the round stuff with the ballnose ,..


Gesendet von iPad mit Tapatalk

[jips]

Same as Tkamsker said , optmise the rough removal with a straight end mill and ball one to remove only what the straight can't last trick is to set the endmill 1mm more than your max depth from the top surface machined to the tool holder to keep the maximum rigidity to the cutter

Envoyé de mon GT-N7100 en utilisant Tapatalk

[johnno402002]

thanks Tkamsker, much appreciated.

[johnno402002]

Thanks Jips, thats a good point on the cutter stick out, I had it out a long way, I'll move the new one up into the collet as you say. I'll rework the operations to use straight end mill to get the bulk of it out.

[mcphill]

Small end mills are fragile. Reducing depth of cut will lower deflection. PAY ATTENTION to the settings and results in GWizard would be my #1 recommendation. It can give good approximate values but you need the right DOC, WOC, cutter geometry, cutter material, max machine HP (go CONSERVATIVE on this!!!). Try to use the largest mill you can to remove bulk material. 4 mm is a pretty darn small cutter. Use high quality tooling - it makes a HUGE difference. Find a local tooling supplier and you can buy professional tools for less than you can get marginal tools online - and you can pick them up same day if you break one.

Keep at it, you are at the flat left end of the learning curve. Not do discourage you, but you have a LONG way ahead of you. Just don't give up, and try to keep the cursing to a minimum

[Tkamsker]

if you send me the IGES file i can do you an gcode as for our machines (are similar to Skyfire just Stronger -
Our envelop is like an Tormach 1100 and we have an 2,3kw Motor so we could go a little faster and deeper ,..

[G59]

so we could go a little faster and deeper ,..

Show us.

[louieatienza]

You cannot use the same stepover on a ball endmill than you do on a regular endmill because of the inherent inefficiency of the tool. The solution would be to decrease the radial DoC or stepover and go from there. Also use the shortest tool that will get the job done.

For roughing, I'd recommend a bull endmill, basically a straight endmill with a tiny corner radius. You would calculate the stepover off the FLAT portion of the tool, not the tool diameter. So with a 1/4" tool with .020" corner radius, you would base your toolpaths on .21" tool diameter.

[louieatienza]

Thanks Jips, thats a good point on the cutter stick out, I had it out a long way, I'll move the new one up into the collet as you say. I'll rework the operations to use straight end mill to get the bulk of it out.

Just ensure you don't push the tool pst the flute fadeaway, or it may not run concentric or at least not fully supported by the collet.

I run my slot depths at half my side milling depths as a general rule. ...

[Tkamsker]

i will but not on this thread this would be hijacking

[G59]

i will but not on this thread this would be hijacking

That's good idea. Just don't forget to post a link or something.

[Hezz]

Hi Johnno,

maybe these machining approaches have been mentioned already but I'm too lazy to read all of the previous posts.

Generally, ball end mills should be thought of as finishing tools taking only a few thousands of an inch off on the last couple of passes. It's best to hog out most of the material with a smaller size bull end mill. You'll need CAM software to do this or it will be beyond tedious. The feeds you can go depend on your machine. The less rigidity you have the slower you will need to go to a point. Also, that looks like a pretty deep cut. It's way too deep for any small mill to handle. For a small mill you should be thinking in terms of .050-.030 of an inch as maximums for depth of cut. That might be even too much for a small mill unless it's really rigid and powerful. So that feature needs to be done in several passes.

Paul

[johnno402002]

Small end mills are fragile. Reducing depth of cut will lower deflection. PAY ATTENTION to the settings and results in GWizard would be my #1 recommendation. It can give good approximate values but you need the right DOC, WOC, cutter geometry, cutter material, max machine HP (go CONSERVATIVE on this!!!). Try to use the largest mill you can to remove bulk material. 4 mm is a pretty darn small cutter. Use high quality tooling - it makes a HUGE difference. Find a local tooling supplier and you can buy professional tools for less than you can get marginal tools online - and you can pick them up same day if you break one.

Keep at it, you are at the flat left end of the learning curve. Not do discourage you, but you have a LONG way ahead of you. Just don't give up, and try to keep the cursing to a minimum

Thanks mcphill, I appreciate the help. I'm using the best cutters I can find locally, they are from Evolute | Faster Machining , sold locally and I have been visiting them quite often lately! You are correct, I do have along way ahead of me, this is my retirement plan, I gave myself two years to come up to speed with it, but the machine arriving a year late has cut that short a bit. I also have a cnc lathe and a cnc plasma cuttter that I'm at same point on the learning curve, plus still working full time in a very demanding job, which is being outsourced.. It's going to be an interesting 12 months ahead.

[johnno402002]

Hi Johnno,

maybe these machining approaches have been mentioned already but I'm too lazy to read all of the previous posts.

Generally, ball end mills should be thought of as finishing tools taking only a few thousands of an inch off on the last couple of passes. It's best to hog out most of the material with a smaller size bull end mill. You'll need CAM software to do this or it will be beyond tedious. The feeds you can go depend on your machine. The less rigidity you have the slower you will need to go to a point. Also, that looks like a pretty deep cut. It's way too deep for any small mill to handle. For a small mill you should be thinking in terms of .050-.030 of an inch as maximums for depth of cut. That might be even too much for a small mill unless it's really rigid and powerful. So that feature needs to be done in several passes.

Paul

Thanks Paul, good advise, much appreciated. I came to the same conclusion on the cam software, after hand writing the first program for the lathe. About 6 weeks ago I bought Onecnc for the mill and the lathe, and it is awesome. But it can't make up for a lack of basic machining experience... The machine is reasonably rigid for its size. I need to rethink the whole machining strategy.

[Hezz]

Thanks Paul, good advise, much appreciated. I came to the same conclusion on the cam software, after hand writing the first program for the lathe. About 6 weeks ago I bought Onecnc for the mill and the lathe, and it is awesome. But it can't make up for a lack of basic machining experience... The machine is reasonably rigid for its size. I need to rethink the whole machining strategy.

Sounds like you are on the right track. You will gain experience with time. Try machining out most of the material about .020" deep at a time. Also, generally unless you have extreme rigidity you don't want to use the full width of the mill. Generally you will step over (sideways) about 2/3 to 3/4 the width of the mill so there is a little area not cutting with each pass. This makes it easier for the chips to be removed If possible.

You will find in the CAM software that there are multiple strategies for material removal. The method can effect the forces on the cutter.

You may be able to redesign the part a little bit to make it easier to machine also. All of the outside dimensions and hole placements can stay the same but if you make the middle material removal area just slightly smaller so that there is a little more of a gap between it's edge and the inside rim of the outer perimeter it will be a lot easier to machine and you will be able to do it with a larger endmill so it will be faster and less likely to break. At least that is what it looks like to me without seeing it in 3D.

[louieatienza]

Thanks Paul, good advise, much appreciated. I came to the same conclusion on the cam software, after hand writing the first program for the lathe. About 6 weeks ago I bought Onecnc for the mill and the lathe, and it is awesome. But it can't make up for a lack of basic machining experience... The machine is reasonably rigid for its size. I need to rethink the whole machining strategy.

I use OneCNC as well. Go on their Tips and Tricks section at the Forum. There are two very excellent articles by OneCNC engineers on how to use HS toolpaths, which include a better explanation than mine about using ball endmills. The articles are stickied to the top. But basically if you use a ball endmill you have to reduce the stepover. Believe it or not, the deeper you go the more rigid the tool is because the closer the top of the work is to the collet. But it will require you to use way shorter tools so that there is minimal clearance between collet and tool.

[handlewanker]

Hi Johnno........whew, you are going in at the deep end..........with a part as complicated as what you have shown I think you need to do a bit of test cutting on something more sacrificial before you get to the final cut on an almost finished one off job and make a mistake.

One thing's for sure........your mill is quite capable of doing a lot more than has been indicated......just needs some practice runs on scrap material to get the feel of the machine.

I would suggest even setting up some hardwood blocs, Redgum or Jarrah are good.... and carving out some random shapes to give yourself time to acclimatise to the mill.

Oh yeah, stay off the coolant for now until you are cutting with some degree of confidence, then increase the DOC and feed rate progressively until you get the feel of it.

BTW, are you writing your own G code or using a CAD/CAM program?

I think a CAM program at the start of a learning curve will put out the best and most economical tool path, but it also assumes you are really into CNC machining and know all the ropes........how does it know if the machine is capable of handling the tool path with the cutter you intend to use.......a ball nose cutter at the best of time is a flimsy tool, although I've used them to mill out various shapes but not with a 4mm diam and lots of stick out with carbide.
Ian.

[louieatienza]

Folks, don't take the bait.....