Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: kolias on November 11, 2012, 05:03:02 PM
-
Finally I cut my 1st Aluminum sample and have some questions. The sample is on a piece 5.5”x4”x1/8” thick and the square I cut on it is 2”x2”. Before this cut I did another sample on MDF and all the cuts on MDF look good (see attached pic)
1. The tool I use for the square cut is 1/4" Drill Point 2 Flute Endmill and the start of the cut is at the top left corner. The speed of the tool is about 6000RPM and the feed rate is 20"/min. As you can see on the attached pic. the cut at the start is not the same as the rest, its deeper and wider. What may cause this?
2. I was expecting the cut to be more sharp and clean but have no experience with Aluminum cuts so is this normal? Perhaps I use the wrong bit?
2. The thickness of the aluminum is 1/8" and I did the square cut with 2 passes of 1/16" each pass but the tool did not go thru. What is wrong here? I set the depth with a zero touch plate so I know that the Z is set properly at 0 on top of the material
3. This is not a question about the cut but I guess the pump I have for the cooling liquid is not big enough to pump the thin oil I use. I control the pump with a momentary switch and when I press the switch the oil just trickles out of the nozzle. Can you recommend a better pump?
-
Others with more experience will chime in. I dont think I would have used a drill pointed (chamfer?) end mill to plunge if that is what you used. I would have used a center cutting 2 or 4 flute end mill which is what it appears you used on the MDF. Are you trying to outline that square or was the intent to cut thru? Depending on the machine and its rigidity the depth of cut might or might not be too much. Did you calculate the chipload, rpms and feedrate or just guess? Dont be embarassed if excitement took over and you just wanted to see something happen! I have broken way too many tools and parts in this journey. MDF looks good. Also dont expect the letters to turn out very well unless it is engraved. They can be much better than what you experienced so far. As you can see wood and metal are 2 different materials. Actually if you were trying to remove the center piece. I would have done a circular or helical ramp into the inside of the line then proceeded. Straight plunges seem to wobble too much for me.
-
Hey Fastest1, thanks for the comments
No experience here, I just used a drill point end mill because I thought it will be the best to straight plunge into aluminum and yes you are right on the MDF I used a 2 flute center cutting endmill.
The intent was to cut thru the square and I didn’t calculate any parameters, I just used what I have gathered from others on the web.
I don’t understand what you mean by "Also don't expect the letters to turn out very well unless it is engraved". I did use a 60deg V bit and although the letters turned out good, I was expecting better.
Also I don’t understand what you mean by "I would have done a circular or helical ramp into the inside of the line"
-
How did you generate the code? Were you just using wizards? Which CAD program are you using? If you used a Cad program generally there are a variety of ways to have your tool enter and exit the stock. You could plunge, ramp, helical (like a corkscrew) and tangential (which I dont understand yet). These different techniques place different stresses and or allow the tool to achieve its depth before following a path to minimize the deflection as you experienced where the top groove was wider than expected. Or maybe they create a place of the chips to be evacuated at the start of a cut. Or a dimple or ridge at a start point of a bore. You also want to overlap if boring a hole or circle to minimize the entry points mark.
That is what I am guessing happened though it could be a few things. So much of this stuff has been counterintuitive to me. Rarely has higher rpm helped me and many times it has overheated the tool, the part etc.
If I am seeing it correctly there are plenty of chatter marks in your letters. This could be caused by many things, fonts, feedrates, gummed up flutes. There is much to learn and engraving will bring new challenges of which I dont have much experince but have made similar errors to you.
Also if the tip of the tool could go all the way thru the material so it uses the side of the tool to cut you would get a better finish on the final cut outs walls. Try doing the cutout with the 2 flute end mill. Also direction of cut is important. Climb milling has produced better results for me though I am getting better at both.
-
I used MastercamX5 but remember I have no too much experience. I don’t want to use Lead-in because the samples I do now are to eventually help me cut the openings / letters for my control panel (8.5"x21"x1/8") and I don’t have a space for Lead-in.
Yes I also see the chatter marks and I think it's because of the wrong type end mill I use. This is the 1st time I do a cut in aluminum and next time I will try a 2 flute end mill as you suggested
-
I meant a lead in for cutting the openings not letters. Do you have a center drill? I was just reading in the "show and tell" section here and there is a thread "bike part" where he uses a center drill for the engraving and has very good results. He didnt think so but i did. The shorter and more rigid the tool, least amount of stickout and w secure workholding will give the best results.
-
Yes the"bike part" post is pretty good, if I can do something close to it I will be very happy, lol
I do have a 2 flute center cutting end mill and will give it a try soon to cut the 2"x2" square. For the engraving I will use again the 1/16" V end mill I have but reduce the RPM perhaps to 2K to 3K and the feed rate down to 15
-
Btw, I too get great results in MDF only to experience some frustration after moving over to aluminum. I also can cut real fast and deep in the wood. But it isn't quite so impressive (it is to me) in metals.
On the engraving hopefully someone else will chime in. I have always understood it is a high rpm tool. At .06125 diameter it should be fast. IIRC engraving is generally a single pass but I could be wrong.
Personally I would take a piece of scrap aluminum. Choose 1 letter. Fix the rpm at 6000. Cut the letter (shallow depth of cut, single pass) at a feed rate you know won't break your tool. Then look at the results. Move over an inch. Reset my X and Y coordinates to 0. Use the feed rate over ride button and reduce the feed rate say 25% and rerun the letter. Does it get better or worse? I am betting this v tool you are referring to ( if it is an engraving tool) is a single flute.
-
The V tool I use is a 1/16" engraving 60 degrees end mill and cuts on both sides of the "V". I know that I have to play with the feed rate and RPM to get a good cut on Aluminum and hopefully I will get there sometimes this week
-
(http://img.tapatalk.com/d/12/11/12/aduquma4.jpg) Just for clarification which tool.
-
The drill point was NOT designed for normal linear cutting it is design to drill a hole THEN lower a touch to get to the flutes and then cut linear.
You need to use a center cutting 2 flute or 1 or3. AS long as it is center cutting for plunge milling . EVEN then plunge cutting takes a very rigid machine to do without crawling around a bit as it plunges.
EVEN the engraving bit must be used at very high rpms because of it tip diam being so small if you go to slow on rpm it tends to drag through the material not cut.
IF you cannot slow the rpm enought you need to go to a smaller diameter cutter. With alum it is ALL about being able to cut with min heat buildup. as soon as the alum gets too hot it gets gummy and sticks to the cutter.
(;-) TP
-
BR, I had posted the pics just for clarification of terms on the tools he is using.
Though I use a drill point all the time for chamfering.
-
One thing to remember IF your machine is not really up to par to do plunge cutting you can always drill a hole where you would normally use a plunge cut. That takes the wiggle out of the equation.
-
I attach 2 pic to show my V engraving end mill + the control panel layout which I want to cut / engrave (this panel is presently made out of plywood to get the machine going).
For cutting the openings I plan to use now a 2 flute center cut end mill at 2500RPM and 7" to 10" / min feed rate
For the engraving I will use the same 1/16" V engraving end mill at same as above RPM / feed rate.
I read in another forum that to much RPM / feed rate develops too much heat and causes the aluminum to "bubble" upwards. Now I don’t know if the RPM / feed rate I said above are ideal but it will be a start point.
-
I am not sure of the bubbling upwards but it will cause gumming up the flutes and breaking the cutter. It will also make some metals harder as it is heating up and tempering it. Perfect your lettering and the like on some scraps first.
-
There ARE feed and speed charts out there in WEBLAND. OR you could the the demo NFW and set it up to see what it recommended for feed/speed.
(;-) TP
-
demo NFW? Newfangled's wizards?
-
yep(;-) TP
-
If you look in Members Docs you will find feed and speed charts for different size end mills along with relationship to material.
Basic good guidelines and if you so desire you can calculate since the basic formula's are there also.
Based on the pic you posted of the V cutter I agree with Terry and would not use it for engraving. Actualy engraving is shallow depth of cut
in my mind. Yours looks more like milling and thus you want to use a small end mill. Carefull since if you have any backlash you can break small ones in a heart beat.
RICH
-
Thank you RICH
-
The results today were perfect as per attached pic and next time I will use even a slower feed rate
Used a feed rate of 10"/min and about 8000RPM for both the square cutout and the engraving.
The cutout was with an 1/8" 2 flute carbide end mill and the engraving with 1/8" V engraving carbide end mill.
Cutting the square I notice that when the tool plunged to the surface was a rough plunge but did a nice job anyway.
Is there a difference between the tool I used to cut the square and a center cutting end mill ?
On the picture I have from a catalogue they both look the same
-
The lower picture looks like a 2 flute end mill, hard to say if it is center cutting however plunging is an aggressive move and on my machines I generally get uncomfortable and flex or deflection seems visible during the action but I dont see it in the results. It might just be paranoia on my part. You might try slowing the plunge rate of that tool, not the feed rate. Otherwise everything looks great. And congrats. Also think twice about slowing the feed down and confirm it in the feed and speeds calculator if possible.
-
Don't plunge, ramp into the cut.
-
Fatest1 you are right, it is just a 2 flute end mill and not a center cutting. I just ordered one 2 flute center cutting and one 4 flute center cutting and I'm anxious to try them. Your idea about slowing the plunge from 15"/min I have now sound good but why you say not the feed rate?
I was thinking to get the feed rate down to 7"/min
Gerry its no problem to ramp into the cut on the samples I do now but when I do the cut of my control panel (see panel picture above) I will not be able to do that because It will not be nice to see the ramp on the finish product (I assume by ramp into the cut you mean Lead-in)
-
No, not lead in. You ramp down to the depth, rather than plunge. Start at the surface and gradually move down while following the toolpath. Say your cutting your square shape. Start at the corner, at the surface. While moving along the first side, ramp down to the final depth, then go all the way around and go over the ramped portion to bring it to the full depth.
-
I could never plunge at 15" a minute with an end mill (not in my present configuration anyway). I would most likely plunge in the 3-4 inch per minute range but I am conservative when breaking tools (that was a joke) my feed rates might be in the 10-16 ipm though I am limited by a 1900 rpm ceiling at the moment. Also as Gerry mentions and I recommended you practice on some scrap, ramping is a form of entry and should leave no marks that arent removed with a finish pass. The helical ramp if used would have been used on the inside of the square, again only noticeable if the small square piece is the part you are keeping. I believe you are trying to cut the panel and the square would be scrap. Same for ramping in along/parallel to your line of cut, the tool should be cutting not dragging and therefore deflecting off path. I only mentioned the feed rate becasue you should stick to what the calculated feed is for that tool and conditions.
-
Not sure what you mean Gerry. For the square, the material is 1/8" thick and I did 4 passes each 0.03125 and the engraving total depth is 1/16" and I did it in 2 passes of 0.03125 each
Otherwise how can I gradually move down? MastercamX5 does not have something like that as far as I know (which is not very much lol)
Fastest I like the 3-4" plunge and I will do it and yes the squares I cut are scrap
-
The lead in will allow you to do just as Gerry is suggesting. I am sure MC has these same abilities if not more. You are running a higher rpm than I can IIRC 8000rpm? so your plunges could be faster than mine but just try to get to depth first and then let the side of the tool do the cutting. When I say square, the cutout that will be scrap (the part right above the word "spindle") could be where the entry was initiated or ramped in parallel a s Ger is saying. Do you ever simulate it, or run it in Mach with the tool above the work or the machine off but running Mach? I do this sometimes due to ignorance of the proper way to a simulation or verify.
-
But Gerry said is not the Lead-in but "gradually move down while following the toolpath" and this I dont know how to do it. Maybe there is a command doing this but I'm now aware of it.
Also I dont know how to define the entry of the tool inside the square (scrap) as you say Fastest1. I select all my squares I want to cut and Mastercam picks a corner on each and does the rest. Dont forget that its not one square to be cut in my control panel so I dont see how this can be done.
I do simulate the cut in Mastercam to assure that all is ok before I get the gcode to Mach3.
-
You could change a few lines of code if your program does't provide for ramping into the material. ie;
G01 Z-........ F.....
G01 X ........ F......
To
G01 Z-.......X.......F....
Which will provide for ramping into the material
RICH
-
Generally if you are selecting a series of shapes (pockets etc) that are going to receive the same machining technique. Though MC might choose the start point and will have a default entry/lead in style. In my understanding which is very little MC is very professional software. I am sure both values are selectable and variable. These are common and accepted practices.
-
Sorry Gerry but now I got it. The toolpath I used is a contour type 2D (default) but within this type there are a few options which I never bothered to investigate. If I click the type button I have a choice of 2D, Ramp, Depth or Plunge etc and of course a few more parameters to set for each type which are too complicated for me right now. As I said I still learn about this program.
I will have to experiment with the Ramp type to see which settings for the ramp angle and depth are good for me before I use this toolpath. Looks like a very interesting toolpath and thanks for the tip
You are right Fastest1, probably there is such a setting which I don’t know it right now. The manual is 800 pages thick and I haven't even scratched the surface of it. Yes MC looks like an excellent CAD/CAM program but since I don’t own it, I just have access to use it for my hobby projects, makes it kind of difficult to learn it properly
-
I am so glad you found those parameters. They will make your results so much better. I didn't and don't expect you to understand MC fully as very few probably do. I have looked at a version or 2 of MC but it was alien to me, I started with BobCad and am now using CamBam too. They each have their little differences in use but likely can accomplish the same or similar results. Progress is being made on your part and soon your results, enjoyment and tool life will all improve. Keep posting as we will all learn.
-
Thru a friend who is knowledgeable with Mastercam I found an alternate way to cut my squares which seems more efficient but requires an extra step which is not a big deal
First I run the simulation to see where my toolpath starts and then I create a point at the start of the cut.
Then I create a new toolpath just to drill an oversized hole at this point, set my Lead-in, and now I run both toolpaths and you can see the results on the attached picture.
Now the tool descents into the hole (on the picture the hole is well oversized for illustration purposes) and does all the cuts using the only the sides of the endmill
-
There are many ways to skin a cat. You are performing a separate drilling op? Though that is a very acceptable method. I can't figure out why you don't ramp into the part. It would minimize the tool change. Sorry I spoke before looking at the attachment. It looks like the tool is going to depth and then a circular lead in, and a circular lead out is being used. That is what I was referring to a while back. It is starting the cut in the scrap side.
-
Actually its a helical entry and not a drilling op to easy out the plunge and I was told that this method is better than ramp. I'm waiting for my new center cutting end mills and then I will give it a try. I also plan to do a sample with the ramp and compare.
-
Both ways are very good at improving cut quality. Definitely try both ways. It is surprising the difference in results, especially small mills not Bridgeports and the like.