Machsupport Forum
General CNC Chat => Show"N"Tell ( What you have made with your CNC machine.) => Topic started by: kcib on July 08, 2013, 10:34:11 AM
-
Hi
I know that this is maybe not the correct place to put this but as there are a lot of people here who are using routers I thought that I might just get a better response.
Anyway I have a problem to which I do not seem to be able to resolve with my router when machining either soft or hard wood and it is now getting very annoying if you look at the picture you will see what I mean I am getting lines which you can clearly see and no matter what I do to try and cure this problem nothing seems to work, I have tried all variations of feeds and speeds but nothing seems to work, I have a solid machine not a small machine that I have built it does not move or vibrate in any way, as you can see by the picture of the machine it is 5 axis and as I say it is all very solid so I am just hoping that someone just might know the answer to my problems and please do not tell me to just sand these lines, these lines are around 0.5 to 0.75mm deep and I have tried machining at all different angles with the grain against the grain etc.
So please help me out here I have not got much hair left to pull out
Thanks
Alan
-
If it were a conventional head I would ask if you had trammed it. The lines, looks to me like it is the placement of the tool and not due to cut direction, wood grain etc. Can you get a close up picture of the lines?
I have sent you a PM
Brett
-
Here is a couple of close up of lines
Alan
-
Sorry about all the pics but it just shows the problems that I am having.
Alan
-
Alan,
What is the cutter size and type (and condition) ?
What is the "step-over" amount set in your CAM ?
What is the milling strategy ? waterline ? or ... ? ?
Might help with diagnostic.
Russ
-
Thanks for your mail, I have just had a phone call from Brett who has given me a couple of things to check out, but in answer to your questions, I am using a new Ball nose router cutter which is 1/8 inch diameter and using a 10% stepover
Thanks
Alan
-
Alan,
You may want include the software as that may be a clue for others to help as well.
Dave.
-
Software used is Vectric Aspire4
Thanks
-
In all honesty, I would post your problem over there as those folks are crazy good with this stuff. ;)
I only have VCarve Pro so I wouldn't be much help here.
Dave
-
Hi Brett
I have done as you asked checked backlash etc. found no problems there and again done as you suggested machined a piece of wood (Oak) then sprayed it back and then re-machined taking off just 0.0200mm (0.0007873992 inch) and you can see the problem with the lines are just top and bottom not sure if that tells you anything that might help?? and because it is a 5 axis machine I did also check that the tool was running vertical etc.
Thanks
Alan
-
Have you tried with the feedrate reduced by about 50%? If so, is it any better?
First, I'd reduce the stepover to 5% and see if it helps.
But to me, it looks like you're getting flex somewhere.
I know you said you have a solid machine, but to me, it doesn't look all that rigid.
Are the grooves always along the same axis? Are you doing a roughing pass first, or a single finishing pass?
-
Is this an actual 5 axis tool path ? ... or just 3 ?
Could it be related to the resolution of the rotary axis's ..... are they fine enough ?
Has this worked fine before ? or has this always been this way ?
-
Aspire doesn't do 5 axis, so I'm assuming it's a 3 axis toolpath.
-
because it is a 5 axis machine I did also check that the tool was running vertical etc.
;)
-
because it is a 5 axis machine I did also check that the tool was running vertical etc.
;)
Because he's using a ballnose bit, being vertical makes no difference as far as the grooves are concerned. The tool is the same shape regardless of the orientation. The only thing being out of vertical would cause would be a slight shift in the location of the carving.
-
Gerry, I was merely pointing out that was not using the 5th axis, that's all.........
-
Alan, If this is the same tool path as in the picture earlier, it seems much better after taking a very light second cut. If that is true I wonder if a third pass (very light) would get rid of all the tool marks. If it does, I would have to agree with Gerry thinking it may be flex. With the bottom of the cut looking so good and only getting the tool marks as you get near vertical makes me wonder if the tool is chipped as RC asked. Dave has a very good suggestion as well about asking Vectrics. A video of the process would be worth a lot.
Brett
-
Thanks
for all the response much appreciated, Gerry why do you say that the machine does not look rigid?? the frame of this machine weighs around 1/2 ton and is as solid as it could be and the sides and the gantry etc. are also very solid! just a bit curious about that, the tool path is a 3 axis was I can see now a bit confusing saying that it was a 5 axis machine, I do a roughing tool path and then a finish path and the finish path cuts at a depth of 0.5 mm (0.01968498 inch) the tool is new so there is no damage to that as for feed rates etc. I have been down to 75 mm (3 inch) per minute makes no difference as for step over have not been quite as low as 5% been down to 8% but will try going lower and see what happens, you make a comment about flex where might this flex be? I can run this machine at some 8 meters (26 feet) a minute and there is no flex/movement anywhere that I can see at that sort of speed not that I ever have or would try and machine anything anywhere near those sort of speeds what I am saying is that if I am not getting any flex/movement at those speeds then at the speeds that I use which for large areas of roughing I might at times go up to 1500 mm (59 inches) per minute and finish speed of 700 mm (27 inches) per minute then I certainly should not be getting any flex etc. anywhere, the gantry and all axis move as smoothly as can be no juddering or jumping around it never loses steps, so can you give me some idea as to where I should look for flex? the spindle motor again there is no vibration or run out it does not lack power (4 Kw - 5 HP) in fact it is way over the top for my needs really, anyway if all else fails I will do as you say and put it over on the Vectric site.
Thanks to everyone.
Alan
-
Try this, put a dial indicator on the table, adjust the dial to zero with contact on the cutter and then push on the side of the uprights.
I am betting you need gussets for rigidity. Looks a little weak to me from the photo. That's why you need to prove it to yourself.
If you were to try different materials with the same gcode program you would get different results of wavy lines. That would prove visually a rigidity or spindle issue. If they were all the same it would be a programming issue.
Edit: Also check with a prybar at the spindle mounts to see if you see movement on the dial, might be a backlash issue on the rotary. I can assure you you have something not quite up to snuff. But cool project thanks for showing it, have fun playing with it.
-
Craig,
Glad you brought this up. I have seen many say the same thing as you, but really give no tolerance for what is acceptable to a particular machine. On your(Craig) machine, if you put a indicator on any of the axis, are you saying it does not move at all? What resolution indicator do you use (tenths, thou, hundred or a metric equivalent ?) and what would you find unacceptable for your particular machine, and most important of all, what's it made of and how's it put together?
I can put an indicator all over the place on my router, and move every axis if I really wanted too. Especially if I use a crowbar ;D
I'm being totally serious, and I'm not looking for an argument, it's just that I see this all time, but nobody ever gives acceptable examples for a wood cutting CNC router table. I personally think there are just too many variables being inserted into each home built table to come up with a standard.
For my own machine, I was a little concerned until I started cutting my first pieces, and then relieved to find that it's cutting to my satisfaction. I possibly should have started a new thread about this, but thought the topic was appropriate here as well.
Dave
-
Thanks for your response Dave as I was just about to write the same thing, if you were to put a dial gauge you could move all the axis and spindle especially if I were to use a prybar ;) I am afraid that the only thing that I would use the prybar for is to smash the machine (joking) as for reinforcing the machine at the points you have marked (Craig) I was already looking at doing this, but the gantry is very solid and believe me I have pushed very hard at where the connections are but I will reinforce it anyway just to make sure.
Thanks for the input all ideas and advice taken on board it is very much appreciated.
Alan
-
Acceptability is based on what you are willing to live with. If it bugs ya, fix it.
That's why they make several sizes of linear rails and shapes. All have a tolerance of their own. Most projects are based on a dream and how much money you can throw at it. A crowbar would develop much more load then most cutters would produce. But if each joint/axis gives ya .002" by just forcing it a little by the time ya get to the cutter tip it might be .006 or more. There is always a sweet spot on a machine & setup. Plus the direction of cut can seen to be better in one axis direction as to others. Learn to program with this in mind. Draw/CAD and write gcode/or CAM to optimize or take in account for what you know are issues you have learned from past projects.
If he was cutting wax it might be a perfect part. I can bet that cutting steel or aluminum it would bark like a wet dog.
As far as my machines (have three mills I built at present, have plans for one more) Each have issues of their own. So depending on the part design, depends on what machine it will go on.
Plus that's what sandpaper is good at, smoothing up little issues. :D
-
Alan, just curious and I'm sure you have checked this already with a dial indicator but are the axis moving the proper distance when commanded to?
Can you run the same shape only keep coming up until the walls have a little step that is absolutely vertical? Or, probably even easier............... can you cut a pocket the same shape (oval) with vertical walls for a test? Make the step down the same as your using in previous programs for step over and the step over the same as well. Make the walls deep enough so that it takes several passes to get to the finished depth....... Maybe 1/2 inch.
Brett
-
Hi Brett
machine does move exactly the distance programmed i.e.if I ask the machine to move 1" inch it moves 1" inch and that is the same for the "X","Y" an"Z" axis , am a bit busy at the moment but will then machine up as you have requested, do you want me to use a ball nose or end mill cutter?
Alan
-
The same cutter you used for the previous parts would be great.
Thanks,
Brett
-
Have just started machining will post a picture once it is finished
Alan
-
Did you say if the grooves were always along the same axis, or do they vary?
Looks like your using an offset finish toolpath. Have you tried a raster finish path?
My machine probably has far more flex than yours, and using Aspire, I've done 3D carvings at 175ipm with no issues. I can probably move my spindle close to 1/16" if I push hard on it.
I don't believe that Aspire is the issue, either. 99.99% of similar type issues you see at the Vectric forum are machine issues. I also happen to be an Aspire beta tester, so have a bit of additional knowledge there.
-
Am using Raster finish tool path, the grooves always seem to be in or around the same area no matter what angle I machine parts from, the parts in the pictures are machined at an angle of 90 degrees, at the moment I am machining what Brett has asked me to do which is machine a pocket into the same shape (Oval) using the same tool, I am in agreement with you on Aspire that is for sure not the problem the problem does lie within the machine somewhere but do not know where else to look at the moment hopefully when I finish machining this part Brett might have some idea.
Thanks
Alan
-
Brett
here is what you asked me to machine it is just under 1/2 inch deep and it has come out without any lines or marks anywhere :) so what does that tell you about the problem??
Alan
-
That the raster based software generated the waves. check your setting on resolution of the created raster file. I set mine quite high so I don't have a stair stepping effect. But I am using ArtCam when I do raster files.
-
That the raster based software generated the waves. check your setting on resolution of the created raster file. I set mine quite high so I don't have a stair stepping effect. But I am using ArtCam when I do raster files.
Do you see the grooves in Aspires preview? If not, then they are not caused by the g-code. Aspires preview is very accurate. If the preview looks good, then your part should look good.
-
That looks good Alan. I would ask Vectric. I wonder if their algorithm has a flaw.
Brett
-
As Gerry mentions, if the preview looks good in Aspire, then it will cut properly. If it's not cutting properly, something is definitely up with the machine(motors, stability, etc).
The reason I told him to go to the Vectric forum, is because those guys are really sharp when it comes to figuring out the source of the issue.
Alan, any chance you have some HDU or just some foam to cut this 3D file in? That would help tell if you have a stability issue as the foam would have almost no resistance.
Dave
-
Thanks guys I know that it is not in the software it is something on this machine it is just finding it, I might well strip down the "Z" axis and remove the 5 axis head unit and fit the spindle motor direct onto the "Z" axis and see if that does make any difference not sure why it would but it is something to try and if all else fails I shall totally rebuild the gantry again but in a slightly different way.
Again thanks for everyone's response.
Alan
-
Alan, Dave has a great suggestion, foam may be the tell all. I would want to know where the problem is before I attacked it. I seriously doubt that Vectrics has a flaw but I wouldn't hesitate asking before I started disassembly.
Brett
-
Hi
I know that this is maybe not the correct place to put this but as there are a lot of people here who are using routers I thought that I might just get a better response.
Anyway I have a problem to which I do not seem to be able to resolve with my router when machining either soft or hard wood and it is now getting very annoying if you look at the picture you will see what I mean I am getting lines which you can clearly see and no matter what I do to try and cure this problem nothing seems to work, I have tried all variations of feeds and speeds but nothing seems to work, I have a solid machine not a small machine that I have built it does not move or vibrate in any way, as you can see by the picture of the machine it is 5 axis and as I say it is all very solid so I am just hoping that someone just might know the answer to my problems and please do not tell me to just sand these lines, these lines are around 0.5 to 0.75mm deep and I have tried machining at all different angles with the grain against the grain etc.
So please help me out here I have not got much hair left to pull out
Thanks
Alan
I use MeshCam Art, and have experienced similar results in the finishing tool cuts. This was prior to installation of the 2010 Screeen Set in Mach3, and was the result of setting the Z Zero after tool change (from the roughing tool, to the finishing tool) by using a sheet of paper as a "feeler gauge". However, as I said, this problem was prior to the 2010 Screen Set in Mach3. Consistent Z Zero settings have been one of the best aspects of the 2010 Screen Set, and accompanying macros. Believe it or not, Depending on the piece, you may actually have occassions, when it is actually desirable to do the finishing cuts "Just a hair shallow", which does result in finished pieces with textures similar to those you have pictured.
-
The Screen Set should make no difference at all when machining I use a different Screen Set to the standard 1024 that comes with Mach and as for measuring the tool after the roughing cut the machine auto measures the tool so that it start in the correct place and at the correct depth so I have no need to use paper / feeler gauge etc. and my finishing cuts are normally around 0.0200 mm (0.0007873992 inch) and on the few occasions a little more.
Thanks for your input.
Alan
-
I'm wondering if your finish cuts are too light? I usually take at the very least .020" (.5mm) in wood.
You may be experiencing cutter flex/machine flex on the roughing run and the finish run is not cleaning it up.
Dave
-
Hi Dave
I have tried taking off more on finishing cuts but it does not seem to make any difference, believe me I have just about exhausted all my options with cutting at this depth and feeds and spindle motor speeds I still seem to get the same results but I have decided that if I do not get any results after I put it onto the Vectric forum then I shall take the complete "Z" axis off of gantry and while that is off reinforce the gantry in the places that I think was Craig suggested then remove the 5 axis head unit and then fit the spindle motor back to the "Z" axis and try again and see what happens if that fails then it might be time for the large very large hammer to make an appearance ;) and see if that frightens the machine into working properly.
Again thanks for everyones input very much appreciated.
Alan
-
You might also check the thrust bearing/play in the spindle motor. There appears to be some vertical deflection as it looks like the cutter is floating up and over the harder grain of the material ... looks like spruce, pine or fir.
If it can deflect over the grain, then as Bud says, it could possibly be floating over the remnants of the roughing cuts.
Hard to tell for sure in the pic, but is there bumps at the harder grain ?
(edit: spelling)
-
... also, machine rigidity is important but the fixturing of the material is too.
Any chance the material is not absolutely secure ?
-
Wood is fixed very securely at one point when this first started to happen I even screwed the work piece to the table just to make sure that there was no flex in wood, as for thrust bearing although this was a brand new motor I did check the bearings etc. just again to rule that out, the wood is that you have in that picture was a very soft pine which is not the best of wood but that is what I had lying around as for the other pictures in this thread that is Oak and I have used other woods hard and soft still get the same problem,
Alan
-
Just a quick update, Gerry asked me if I had machined the wood using the offset option and that I should try the raster option but as I said I was machining using the raster option so today I thought that I would have a go at machining just a dish shape using the offset option and I thought that all was going well until the end when I noticed that I had some horizontal lines at the top and bottom of the dish so I done two more finish tool paths going down a further 1mm (0.03936996 inch) and although it looks better the lines are still there and it just seems weird that the lines run parallel when the part is machined in circles, take a close look at the picture the lines are not that bad now but I have machined the part 4 times to get it like it is now, also what seems strange is that the lines appear at the top right of part and the bottom left the arrow shows the direction tool was cutting.
-
To improve the finish cuts, what I have done is to increase the resolution (stepover). MeshCam Art has an option to use Adaptive Stepover, which does result in a better finish cut. However, it also results in an increase in cutting time. I just finished a piece, which is Old Glory flapping in the breeze. The total cut time for that piece was almost 18 hours. But it did turn it pretty nice. I will post a picture later.
-
the lines are still there and it just seems weird that the lines run parallel when the part is machined in circles
I'm almost certain that this is a mechanical issue.
Looks like your machine is rack and pinion? Check that the pinion has zero play, and check it in several different spots. Are the Drives from CNC Router Parts by chance? I've read of multiple instances of their pinion bushings wearings and becoming sloppy.
My guess is that the probllem lies in the axis along which the red arrow is pointing.
-
Yes it is rack and pinion and have checked for any play in it but have found it to be spot on and no the drives did not come from them, the arrow is pointing towards the "Y" axis so I will check all racks etc. later today as it is very late now and it is past my bed time and I do need some sleep right now, will let you know if I find anything.
Thanks
Alan
-
Gerry
I took what you said on board and checked out the rack pinions for wear/backlash and could not find any problems there but I did have on the shelf some unused pinions of the same size but instead of being metal they were made of Glass-filled Nylon so I machine and fitted them and was quite surprised just how quiet they made the machine not that it was noisy in the first place but then came the problem, her indoors you know the one she who must be obeyed needed some help so never got round to finishing yesterday so have finished it off today and set about machining a basic 3D model done the roughing and finishing using the raster option and the same tool for both and was dismayed to fine that I still had lines very similar to the ones in my very first post on this problem but a lot fainter, so then I just decided to do a finish tool path(over the same part) but this time I used the offset option again using the same tool and you can see the result, perfect no problems at all doing it this way so tried again using the raster option but still get lines but as I say a lot fainter than before so I can live with that and just sand those marks away so not sure what happened by fitting the new pinions but it seems to have done the job so now I am very happy ;D.
A very big thank you to all who had some input into this and to Gerry who gave me eventual answer.
Many thanks
Alan
-
Is your rack and pinion direct drive, or do you have a reduction?
It would appear that the issue is due to the meshing of the rack and pinion.
-
It has a reduction drive on the machine 4:1 ratio
Alan
-
Gerry
I am just done another program using Aspire and am doing the roughing cut using the "Z" level strategy and am using the Raster for finishing cut at a 315 degree angle and so far no lines have appeared will let you know what the result was like when finished, also had a look at the meshing but cannot see any problems there but after I have finished this job I shall take another look just to make sure there is nothing there.
Alan
-
Have just finished machining this and as you can see in the picture there are still lines if I machine this way, it was machined from bottom to top at an angle of 315 degrees using a brand new 1/8 inch taper ball nose cutter that I bought from USA (Think and Tinker) I am now going to go and check the meshing as you have suggested (Gerry) the lines at the bottom of part are not very visible on picture as the wood there is lighter that the other side.
Thanks
Alan
-
I love my two sets of Festo clamps
-
Yes very good but not so cheap to buy here in the UK.
-
Somewhere over $100 here for a set, no discounts either. I bought mine a couple of years ago, first set came with the folding work bench. I have several Festo tools LOVE them all. Their straight track guided circular saws are awesome. What a great system to cut large panels out of larger sheets. Adjustable speed, straight, clean cuts every time.
-
Late to the party, but might as well throw in my two cent worth. I see the Kitchen (http://en.wikipedia.org/wiki/Vance_Miller) sink has already been thrown. Looks like lash to me. The problem areas being 180 degrees apart is usually a tell-tale sign of lash. The reason why most of the ridges are gone when doing a very small step-over, or fine finish cut, is because there is most likely not enough force to shift the machine from one side of the lash to the other.
Also, I would definitely brace the gantry, as stated before. It's a simple procedure, CHEAP, and if it don't help it, it certainly won't hurt it. Regarding the indicator and flex, that should give you a good "before and after" measurement. You will never get all the flex out of it though. I can put an 0.001 indicator in a bridgeport spindle and get lots of needle movement with not much hand pressure at all on the spindle, or the table, or any other moving part. Everything needs clearance to move.