Another Tool Chatter Post

[MetalShavings]

I've been asking around in places where I thought I might have the best chance of getting a good answer or even some suggestions on how to go about dealing with tool Chatter on inside corners. Back when I first bought my Tormach 770 I could swear I came across a video tutorial that explained what I might be able to adjust within the SprutCam software to change the feeds and speeds or WOCs/DOCs in order to mitigate or stop the chatter when my end mill got into those inside corners. I contacted SprutCam USA to ask if they had put out such a video but it turns out they had not; at least according to the guy who replied to my query, and to the best of his knowledge neither they nor Tormach had put out any such video.

I also contact Tormach about this but they never got back to me.

So I'm wondering: The HSM tool paths I'm currently using are working extremely well for me using the HSMAdvisor generated feeds and speeds; that is, until my end mill reaches those inside corners. Then I get the finger-nails scratching across a calk-board chatter that drives me nuts. It only lasts a couple of seconds each time but still, it can't be good for the cutting tool or my machine and it certainly doesn't do my surface finish any good although I do leave some material for finishing passes with a smaller end mill.

I wanted to ask you guys with more experience with these things; have you come up with a method of dealing with chatter on inside corners? I have a general understanding of the cause of this chatter and I have taken steps to mitigate it all together but to me it entails one or two more tool changes and if possible I'd like to allow the 1/2" end mill I have been using to continue its roughing tool paths without having to stop each time it comes to an inside corner. I have to note here that I actually have gone to a smaller diameter end mill to help stop the chatter but this adds time to the overall amount of time that it takes to machine the parts in question. Also; I know that I can run a drilling tool path before hand at each of the corners to help mitigate this chatter as well but, I'm hoping one of your guys knows your SprutCam software intimately enough to suggest a possible way to tweak the G-Code so as to not have to add any more tool changes to the running of these parts.

It's been a long while since I viewed the video I mentioned above but, If I remember correctly, the guy in the video I alluded to did something to the G-Code by going down the column on the left of the SprutCam screen toward the bottom where it listed the faces or the edges to be machined and he changed a few of the numbers there which effected either the WOC or the spindle speed. This was back when SprutCam 7 was all that was available. I still use the highest version of SprutCam-7 and I don't really want to spend any more money on upgrades and such if at all possible.

Does anyone remember seeing such a video? Is anyone SprutCam-Savvy enough to figure out a work-around within the G-Code itself for dealing with this kind of chatter? The guy from SprutCam USA that replied to my inquiry seemed more about upselling me the latest version than really offering any suggestions with the SprutCam version I'm working with now. So I'm asking you guys.

Crossing my fingers.

MetalShavings

Similar Threads:

• Crazy tool vibration/chatter, can't figure out why
• Need Help!- Trying to get rid of tool chatter
• Strange chatter on part off tool
• Parting tool chatter fix
• Seco Tool getting chatter on Aluminium

[SCzEngrgGroup]

Any good HSM CAM should allow you to specify a different feed rate to use within a specified distance from an inside corner. That will largely eliminate chatter in the corners. I don't know if SprutCAM supports it or not, but HSMWorks/HSMXpress/FusionCAM does.

Regards,
Ray L.

[zero_divide]

Hey man,

I know you pasted on my forums inquiring about the same and I even gave you an answer... But I did not realize you were having problems with HSM roughing.
Somehow I thought it was the finishing.

Any way. Here is the recipe: set the minimum toolpath radious to something like 0.05" and this will entirely remove all sharp corners in your toolpath.

I do not know where it is set up in Sprupt, but I know it is in MasterCam's toolpath parameters, so i thought it would make sense to have it there as well.

[IMT]

Metalshavings,
I've been using Sprut7 since 2010, haven't seen the video you speak of and don't know of any way to control speed, feed or WOC specifically for inside corners. I don't know everything about Sprut but have never come across such a feature. Pocketing efficiently with Sprut has always been a challenge, the HSM tool paths are just not very good. When I cut a pocket that has .250 inside radius corners with a .500 endmill, the best approach i've found is to helical plunge a .600 dia. hole that is tangent to the faces (minus finish allowance) followed up with a vertical plunge that is .005 offset from the corner center. Then rough with your normal tool paths and parameters, no chatter in the corners because the material has already been removed. Takes more time to program and run but can all be done with the same tool.

[MetalShavings]

Hey man,

I know you pasted on my forums inquiring about the same and I even gave you an answer... But I did not realize you were having problems with HSM roughing.
Somehow I thought it was the finishing.

Any way. Here is the recipe: set the minimum toolpath radious to something like 0.05" and this will entirely remove all sharp corners in your toolpath.

I do not know where it is set up in Sprupt, but I know it is in MasterCam's toolpath parameters, so i thought it would make sense to have it there as well.

Thanks Eldar:

I'll give that a try. There is a text field in the SprutCam strategies page that may allow for such a thing. In fact I believe I've used that particular text field before in order to get the circular cutting paths of my end mills to cut in larger circular patterns but if I go to high, it fails to produce a tool path at all. I believe it's called "Corner-Smoothing" but I'm not sure. No matter, at this point I'm willing to try anything to get that chatter to go away.

MetalShavings

[SCzEngrgGroup]

When I cut a pocket that has .250 inside radius corners with a .500 endmill, the best approach i've found is to...

Chatter is almost unavoidable if the corner radius is equal to the tool radius, because you suddenly go from contact only along one side of the tool, to contact across 90 degrees of the tool circumference. When cutting inside corners, always make the corner radius larger than the tool radius. When using a 1/2" tool, I'll make the corner radius at least 0.27", and still slow down quite a bit beginning shortly ahead of the corner, and ending shortly after the corner, to avoid chatter, because even with the larger radius, tool engagement still increases significantly going through any inside corner where the radius is not much larger than the tool diameter.

Regards,
Ray L.

[IMT]

Chatter is almost unavoidable if the corner radius is equal to the tool radius,

Absolutely true. Increasing the radius to .270 with a .500 dia. tool is only marginally better.
This is why I plunge cut the corner. No chatter in the corner because there is no material being cut.

[C*H*U*D]

770 + .250" radius + .500" endmill = bad things.

The 770 is a triathlete not a power lifter. Let it run with a 3/8", 3 flute and I bet you can take your fingers out of your ears when it enters a corner :-)

This is probably not the answer you want to hear, but Ray and IMT are right...if you really need to have a 1/4" radius, then decrease your tool size. If you really need to run a 1/2" tool then increase your radius. I rarely go above 3/8" with my 770...I'd rather let it run a higher feed rate than push a heavy cut. At 660lbs, the rigidity is just not there on the 770.

[MetalShavings]

Chatter is almost unavoidable if the corner radius is equal to the tool radius, because you suddenly go from contact only along one side of the tool, to contact across 90 degrees of the tool circumference. When cutting inside corners, always make the corner radius larger than the tool radius. When using a 1/2" tool, I'll make the corner radius at least 0.27", and still slow down quite a bit beginning shortly ahead of the corner, and ending shortly after the corner, to avoid chatter, because even with the larger radius, tool engagement still increases significantly going through any inside corner where the radius is not much larger than the tool diameter.

Regards,
Ray L.

The radius of these particular inside corners is .276". I still get the chatter I mentioned for the reasons that you've listed. The problem here is that the feeds and speeds that I'm using with the 1/2" end mill are working so well that I hate to mess with them. It's those dang inside corners that drive me nuts with the chatter.

All the comments posted thus far make absolute sense from a machining stand point. The thing I was inquiring about is the possibility of adjusting either the feeds and speeds or the DOC's within the G-Code itself through the SprutCam software. It appears that this is possible with some of the high end HSM/CAM software but not with SprutCam unless you upgrade to their latest version which includes some type of "Adaptive-Compensation"; whatever that means.

Unless I win the lottery I won't be upgrading my SprutCam software so I'll will be trying out the suggestion that Eldar/Zero_Divide made. If I do win the lottery any time soon I'll most likely buy the higher end CAM software but for the time being, If I can tweak the "Corner-Smoothing" feature in SprutCam so that it keeps my roughing end mill from going into those tight corners in the first place, I'll be happy to just let my smaller cleanup end mill quietly round out those inside corners.

Thanks to all who took the time to post suggestions. I don't want to sound patronizing but they did all make sense. Most of them I had already tried but I was wanting to try to find a fix that didn't entail additional tool changes or major alterations to my existing G-Code. It's funny but I've found that the problems I encounter in this hobby all seem to have an easy fix. It's finding that easy fix that's the hard part.

MetalShavings

[SCzEngrgGroup]

The radius of these particular inside corners is .276". I still get the chatter I mentioned for the reasons that you've listed. The problem here is that the feeds and speeds that I'm using with the 1/2" end mill are working so well that I hate to mess with them. It's those dang inside corners that drive me nuts with the chatter.

All the comments posted thus far make absolute sense from a machining stand point. The thing I was inquiring about is the possibility of adjusting either the feeds and speeds or the DOC's within the G-Code itself through the SprutCam software. It appears that this is possible with some of the high end HSM/CAM software but not with SprutCam unless you upgrade to their latest version which includes some type of "Adaptive-Compensation"; whatever that means.

Unless I win the lottery I won't be upgrading my SprutCam software so I'll will be trying out the suggestion that Eldar/Zero_Divide made. If I do win the lottery any time soon I'll most likely buy the higher end CAM software but for the time being, If I can tweak the "Corner-Smoothing" feature in SprutCam so that it keeps my roughing end mill from going into those tight corners in the first place, I'll be happy to just let my smaller cleanup end mill quietly round out those inside corners.

Thanks to all who took the time to post suggestions. I don't want to sound patronizing but they did all make sense. Most of them I had already tried but I was wanting to try to find a fix that didn't entail additional tool changes or major alterations to my existing G-Code. It's funny but I've found that the problems I encounter in this hobby all seem to have an easy fix. It's finding that easy fix that's the hard part.

MetalShavings

You might consider ditching SprutCAM for Fusion. For small users, it is free, and includes excellent 2.5D CAM. If you need 3D CAM, that does come at a price. Fusion will easily import models in all common file formats (Solidworks, STL, IGES, etc., etc.). FusionCAM lets you easily slow down in, and near corners.

Regards,
Ray L.

[Steve Seebold]

First off, corner chatter depends a lot on the flute shape of the end mill you are using.
Second would be how fast you are spinning the cutter and your feed rate.
Third would be the size of the cutter in relation to the finished pocket.
Fourth would be how much stock you are leaving for your finish pass.

I would be using a 3/8 end mill to cut a .276 corner radius.

If you leave .025 on the part for finishing, you're going to make over
90 degree contact when you come to the corner and on these light
machines that "will" chatter.

[popspipes]

How the part is clamped will make a difference as well, it needs to be very ridgid.
I solved a chatter issue I had by just changing the way it was clamped to the fixture.

[mountaindew]

You might consider ditching SprutCAM for Fusion. For small users, it is free, and includes excellent 2.5D CAM. If you need 3D CAM, that does come at a price. Fusion will easily import models in all common file formats (Solidworks, STL, IGES, etc., etc.). FusionCAM lets you easily slow down in, and near corners.

Regards,
Ray L.

Anything Fusion can do "A very new program" Sprutcam can do 5 different ways with 150 different options to tune and adjust those 5 different ways all on 150 different types of machines. The user needs to look at all the options and choose the way they like or want to get the job done!

To help the op.
Try smart feed if you think that will help. Trapping cutters at any speed is not my way of machining "to noisy" and others have mentioned this above.
Under strategy try setting inner corner radius to larger then your cutter. Then go back and setup one of 9 different rest machine operations that are designed just for this problem.
Or I could name a dozen more ways to avoid this problem and you dont have to change cam systems.
Just trying to help.

[Uman]

First off, corner chatter depends a lot on the flute shape of the end mill you are using.
Second would be how fast you are spinning the cutter and your feed rate.
Third would be the size of the cutter in relation to the finished pocket.
Fourth would be how much stock you are leaving for your finish pass.

To this I would add your choice of cutters; all cutters are not created equal or optimum for your particular mill.
I found the IMCO Streaker justs zings in aluminum. When other cutters would chatter, the Streaker was rock solid; it seems to be much more tolerant, stable and capable of much more aggression.
Minimize your stickout and hammer down.
On a side note, I discovered one of my ER20 collets was also a chatter culprit.

[Steve Seebold]

The ER20 holders work great if you're drilling
holes but they're just too long to use with big
end mills.

The longer they are, the more they'll chatter.

[SCzEngrgGroup]

Anything Fusion can do "A very new program" Sprutcam can do 5 different ways with 150 different options to tune and adjust those 5 different ways all on 150 different types of machines. The user needs to look at all the options and choose the way they like or want to get the job done!

To help the op.
Try smart feed if you think that will help. Trapping cutters at any speed is not my way of machining "to noisy" and others have mentioned this above.
Under strategy try setting inner corner radius to larger then your cutter. Then go back and setup one of 9 different rest machine operations that are designed just for this problem.
Or I could name a dozen more ways to avoid this problem and you dont have to change cam systems.
Just trying to help.

There are MANY reasons to at least LOOK at Fusion, even apart from the OPs original question. The HUGE advantages of integrated CAD and CAM should not be under-estimated - I would NEVER go back to a non-integrated system, as it is a MASSIVE time-waster. And the CAM in Fusion is very highly developed and capable, as it is, internally, identical to HSMWorks, an $8K+ CAM system which has been around for a LONG time, undoubtedly has a larger user base than Sprut, and it incredibly capable. In fact, HSMWorks was one of the pioneers of HSM! I've been using it for 4-5 years with great success. The CAD side of Fusion has a few rough edges, but is still still excellent. I used Solidworks for 4 years, at a total cost of over $8K, and this year I have abandoned Solidworks entirely in favor of Fusion. Fusion gives me everything I need, and a lot of things my Solidworks license did not (including extensive simulation capabilities, like FEM, Thermal, etc.). I've had few problems, none really significant, and the CAM is the highlight of the whole system. And all for a whopping $300/year. FWIW - I HAVE used SprutCAM. Well, tried to, and rejected it for a host of reasons. I consider FusionCAM to be head and shoulders better than Sprut, in every way. Not least of which is their support forum, which would have given the OP the answer he needed in, quite literally, minutes.

Regards,
Ray L.

[MichaelHenry]

Under strategy try setting inner corner radius to larger then your cutter. Then go back and setup one of 9 different rest machine operations that are designed just for this problem.
Or I could name a dozen more ways to avoid this problem and you dont have to change cam systems.
Just trying to help.

Thanks for that - that's one of many Sprut parameters that have confused me as to purpose over the years. Sprut could really use a version of the manual that was written in understandable English.

[AUSTINMACHINING]

This may or may not help but it's a very good description of how to avoid trapping the cutter.

[MetalShavings]

Thanks for that - that's one of many Sprut parameters that have confused me as to purpose over the years. Sprut could really use a version of the manual that was written in understandable English.

If I remember correctly, there are actually two different text fields within that particular "Corner-Smoothing" area of the Strategy page. I've been fiddling with the upper one because I read that the lower of the two text fields applies only with 2d tool paths. I read this when I clicked on the "Help" icon for the Strategy page.

Which of the two are you referring to? I found that varying the "Corner-Smoothing" upper text field seems to do very little when it comes to inside corners. If it's a larger area that's being milled with circular cutting paths, the upper text field will cause the end mill to run in a larger diameter cutting path but still, when it gets to those inside corners, out of necessity, the end mill can't spin in those larger diameter cutting paths any more. It has to tighten the circular cutting paths to accommodate the tight quarters.

My written descriptions may be causing some of you to conjure up pictures in your mind of conventional inside corners like one would expect in a rectangular pocket. In reality, it IS a type of pocketing tool path but there are no true inside corners per-se; just tight areas within that tool path. I guess it's all the same though regardless of how it's described. I'm still getting the finger-nails scratching across a chalk board chatter; at least with the 1/2" end mill I was using. Now that I'll be using a 3/8" end mill to run those same tool paths I'll find out if it make a tangible difference in the chatter. In the mean time I'll have to play around with both of those text fields within the "Corner-Smoothing section of the Strategy page; as well as the "Rest-Machining Operations." I've never played around with this feature.

I have a little time to experiment. I won't really need to run another batch of these parts until I sell of my present inventory. It will be a while. This is time I can use to find the fixes that will work on my machine cutting these tiny parts out of 1018 steel.

MetalShavings

[mountaindew]

Have you ever even tried Fusion, and its CAM? If not, perhaps you [should give it a try and get] first-hand knowledge of the product.

Regards,
Ray L.

You have great knowledge about this subject and I respect that.
I was trying to help the op and avoid telling they need new anything like software, machine or cutter. Like others mentioned above its not the software for the most part its the problem and how you deal with it. Sprutcam is not going to automatically avoid cutter trap, maybe it will in future release. Some companies get feature feed back by reading how others use their software on forums.

As for software in general I can claim to be a power user on almost any program ever written. Why because I have used and written software beginning with a vax 11780. My first computer ran msdos 1.01 and I still have the floppy disks in a frame on my wall. I understand 6 programming languages including assembly language. I found Sprutcam easy to use because I understand the compiler its written with. And the predefined dialog boxes, data tree structures it uses and even the object oriented programming language including the data inheritance structure it uses. I can even spot errors and know why they are there So when you know whats under the hood of the car its easy to drive it.

As for Fusion I have owned stock in adsk for a dozen years , giggle. And used Autocad to draw buildings since around 1993. version 3.0 I think and it cost the company $2k, and all acad did back then was draw vector lines, text, dimension and scale drawings for plotting. Had a 15k$ plotter that was 5 feet wide behind me against a wall and a 5k$ 3ft x4ft calcomp digitizing tablet in front of me for 15 years. Not my first rodeo with cad software giggle.