Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: Overloaded on December 27, 2010, 09:17:15 PM
-
Hey All,
Pic is the top view of 4" x .5" thick alu. (may need some of 1018 steel also)
The parts are identical, just rotated to save material. (I'm Scotish.... ish :).)
I thought about drawing the basic profile in 2 layers. One to cut the majority (blue), and another to cut it off (Yellow).
I imagine a .250 endmill, several passes.
How would this normally be done in the real world.
Thanks
-
Does those parts needs holes.
If yes, I would drill the holes first and bolt the part on a setup plate.
Also depend how many you have to do.
Will not be the same setup for 4 parts as it would be for a thousand parts.
You could leave some tabs to keep the part in place and avoid breaking your end mill or damage the part.
Is the distance from part to part in the X direction is the same as your end mill diameter.
Jeff
-
First, I would have to ask what level of accuracy your wanting. If their for "farmer Joe" to weld up on his tractor equipment, I would just hang 'em off the end of the vise, cut the profile as best I could, knock 'em up against the belt sander and send them on their way. Otherwise, I personally would not do them all in one big stretch like you have them laid out. If you think along the lines of "2 parts per setup" then you will still maximize the material usage, as indicated by the green vertical line in the pic. Like Ostie said, if it has holes, (more than one, preferably) that's really an advantage, and is going to be your easiest method. Just bolt it to a setup plate using the holes, and then you can cut around the entire profile. Sometimes, I have drilled the holes smaller than required, in order to make a closer fit around the bolt(s), or even ream them for shoulder bolts, and then after the profile is cut, go back and drill the holes to the required diameter. If it does not have holes, I would cut the plates along the vertical green line in the saw, leaving yourself a small bit of extra length for the next operation. Next, put one part in the vise, and square up one of the ends with an end mill. Flip part, square up the opposite end. Rinse and repeat for all the parts. Next, I would discard the vise, or move your operation to the side of the vise, and cut the profiling operation on the milling table. First, find a sacrificial plate, so you can cut the entire depth of the part, without ruining your table. Then square up the part along the table, by using the end you previously squared up as your guide, and hold down the part using a toe clamp or similar. Use an edge finder to get your X zero point. Looks like you have some extra meat in Y, so you might get by without the edge finding in Y, using a guesstimate. Cut along your blue and yellow lines. Flip part around, repeat.
Obviously, "the devil is in the details" as they say, and methods will vary greatly. Everybody has different tools and machinery at their disposal(or lack thereof), along with personal methods.
-
Hi guys,
Jeff, there is one hole, cant add another so I figured it wold not be any good for holding, just locating maybe.
I do about 30 pcs each run.
I also thought about tabbing but would like to eliminate the clean-up afterwards.
I can space them in X as necessary to allow a finish pass at full depth for a good finish.
I like the idea of "pairs" Sam, that looks to be the simplest and is what I will plan on using for now, THANKS !
There is a little extra material in the Y so that makes it easier as you say.
This is not a super critical part as far as the profile goes, they are part of a weldment. But I would like for them to be within +/- .005"
Thanks again men,
Rc :)
-
What is the hole size? If it's big enough to put a substantial bolt in it (like 1/4"), then you're good. Bolt the stock down to a sacrificial plate (use enough for a pair like Sam suggested - you will have two bolts holding the stock), using the holes, then mill the profile leaving about 0.01" for the last pass - it is enough to hold the stock, but yet not to much to develop large cutting forces on the last pass, so the single bolt per part should handle it fine. Just tighten it firmly.
Dan
-
Another good idea, thanks Dan.
That would let me cycle 2 parts per set-up.
I like it.
-
And, you wouldn't have to mill the ends square after you cut the stock, since you can cut the entire profile, so that's also a step deleted.
-
you have one long straight edge on the part. Align it to a finished edge of the material so it does not have to be cut then clamp each part from that edge and then push the button and cut as many as you can line up at one time. IF material waste is a concern then alternate the part to the upper and lower edges
Just a thought, (;-) TP
-
Hi T,
The part is 3.8" by 4.1" The material is 4"
The long straight edge cant be used as the part would not fit the material if rotated 90 deg.
The only common straight surface is the small one at the bottom of the 1st part, which is too small for a hold-down.
Also, the "ear" at the top is actually a radius, same rad. pt. as the hole.
If I had wider material, your method would be perfect ! Just trying to use the matl. that I have on hand.
Thanks Terry
-
lay the part down so the long angled line lines up with the bottom of the material, then rotate the next part so the angled line uses the top. That gives you a clamping spot that does not have to be machined.
Looks like it would work from here.
Do you have a dxf of the part, I will lay it out here to see if it fits.
Just a thought, (;-) TP
-
This is very close to what it will end up being.
Thanks MUCH !
-
Similar to this TP ?
Only 2.8" wide tis way. Could use 3" stock !
Rc
-
THis is how I would do it.I do a LOT of small batches for the locals. Make the batch as big as will fit on the machine. The trick to making $$ on small batches is do as many as possible per setup.Then make it hands off to do each setup. Rather than drill the holes (extra tool change) just mill out the holes with the same tool you do the rest of the profiling.
(;-) TP
HECK you already figured it out Good Job (;-)
-
Beautiful !
I'll try to rotate and pos 4 places in CAD, might need some help there.
Generating the tool path should be no problem.
The hole is .511 +/- .001 so I will have to drill & ream it separately.
At least I'm on the right track.
Thanks TP
-
You could go ahead and mill the hole to -.008 that leaves you enough to ream.
Let me know IF you need more help, (;-) TP
-
Will do,
I managed to get the copies to snap where I wanted them then removed the "finished edge" vector. (just guessing at this but it look OK)
6 at a time.
This pattern works real good on 4" material. Less waste thanI expected.
It will mill the holes undersized. My machine is a bit sloppy. What the heck, only 1 tool change. It's fun to watch.
I made the tool path with Sheetcam but it exceeded my eval limit.
Have to try LCam ..... ( it's OK, I've got drugs).
Thanks TP
-
1 drawback to this method that I see is if its drawn for 4" wide material, the material MUST be exactly 4" or half of the parts will be off.
An advantage of Sams method, all parts will be identical regardless of the material width as ther is excess all the way around.
Still though, this "6 pack" method would be accurate if I did the 3 profiles along the reference edge, then unclamp and rotate the blank and do the other 3. It would be about 20" long, Would only need 4 clamps this way too.
Thanks men.
-
Hi Terry,
Good idea as always! I like your productivity.
Russ, do as Terry suggests for a stock you have and then it is fairly simple to tweak the G-code to accommodate for future stock changes. Let's say you do your G-code for a 4" wide stock - bottom parts aligned with the bottom edge, top parts aligned with the top edge. Be sure you first cut all the bottom parts and the move to cutting all the top parts. Let's assume next time the stock you get is 4.1" wide. You align the bottom edge of the material with the bottom parts' edge and the bottom parts are fine. Now the problem is with the top parts. Use "G52 Y0.1" before the code for the top parts. It will offset the coordinate system by that amount. Program "G52 Y0" in the end to cancel it.
Dan
-
Oh... one more thing. I am not sure how it works with G41/G42 offsets, so be careful if you're using them. Sometimes G41/G42 offsets don't like offseting of the coordinate system.
Dan
-
G52 .... perfect !
Thanks Dan.
Will watch out for the 41/42 anomalies but I don't think the cam uses them.
Nice tip, hope I can remember it for use in the future.
-
OK, that wasn't so bad. Didn't really want those old 1/4" endmills anyway. ;)
They proved to be a little light for .375 steel plate. 3/8" endmill worked much better.
I decided to run these 1 at a time and used the same basic method Terry mentioned, I didn't want to risk scrapping 6 per setup. Glad I did ! ::)
Held the stock in the vise and put a clamp on the part so I could run a finish pass. Then flip and repeat.
They came out better than I expected. Even the hole is almost acceptable but will ream them anyway.
Perhaps you could help me with the feed, speed and depth of cut.
The rpm dial on the head is pretty well hosed so I'm just guessing at the actual rpm. I do have a handheld digital tach that I can use until I get an index pulse to Mach.
Using a 3/8" (9.5mm :)), 4 flute, HSS endmill.
No coolant hooked up yet, VERY soon though. Just a spray bottle w/ soluble mix for now.
I ran these , DOC .100" and tweaked the rpm and fr ( 2 to 6 ipm ) as I went along trying to get it done as quick as possible.
What would you guys recommend as a starting point ?
DOC
RPM
FR
Thanks
-
Russ,
This link can calc what your asking.
http://www.custompartnet.com/calculator/milling-speed-and-feed
There are other sites as well. I usualy just use the info or charts that are in Cleveland Twist Drill / end mill technical section. It provides a good table for chip load to rpm and is easy to use.
Sometimes nothing beats the good old paper sheet in hand.
RICH
-
Thanks RIch, the info you posted reflect pretty much what I see elsewhere.
It all seems soooooo fast to me , just looking at the #".
I'll just tinker with it. Thank goodness there's a sale on endmills this week.
Beginning to think my .100" depth is too great.
See ya.
-
Hi Russ,
Looks good.
If machine rigidity is not a problem, these end mills should do fine up to depth of 1/2 their diameter cutting full width.
If you can get a deal on some roughing end mills it would save you some money on the finishing ones which you want to keep sharp. Also roughing end mills can go as deep as their diameter on a full width cut. Carbide are best and are a good investment, especially when you have no coolant.
Dan
-
Thanks Dan,
How about the chips ... will they destroy a carbide cutter if they are not blown clear of the slot ?
I'm thinking of getting a mist type deal with just enough air to keep the chips outta the slot but not blow them all over the shop.
Anxious to try the carbide.
See Ya,
Russ
-
Russ,
Good evacuation of chips is certainly desirable. I haven't investigated how they effect the tool life, but they sure cause an awful noise if not evacuated to clear the cut. Just hearing that noise makes you think it's going to break the cutter, so haven't had the courage to leave it like this for more than a few seconds ;)
Dan
-
I've always seen it as a must to get the chips out, especially with carbide, because they have a tendancy to chip. Once they start chipping/fracturing, it goes downhil fast.
I do most of this kind of work manually, and depending on the size of the job, I just use a handheld blowgun with quick blasts of air, or set up a mister without the coolant to keep the chips out. Unfortunately, this throws chips everywhere as we do not have enclsures around our mill. Whatcha gonna do :D
Dave
-
I did hold my blow gun at the cutter with just enough to clear the dry chips and it took surprising little velocity/vol to keep it cleared. Didn't make much mess at all.
No encl here either. Maybe on next mill tho.
Dry air with carbide will be my next attempt, then maybe mist.
Tanks Dave.
York this year ? :)
-
I use a a shop vac to take the chips away along with a cutting fluid ( hand sprayed / too lazy to add a drip nozzle ). Nothing auto in my hobby shop.
Don't like the air spray since the chips go all over the place and not good fom a safety point of view ( they would fire you if you did that at the company shops ).
The roughing end mills are great for fast material removal especialy in Al.
Over time i have read a number of technical books on milling. Cincinnati Milacron had a book alll about the testing they did with end mills and the SME continues to research
with member companies. That said, there has been advances in tooling etc and a lot of the companies have tech info. After a while you find it's just automated in a some program and refined
particular info is presented. Same basic rules with the clarifier to adjust based on testing of your machine, material, etc.
Thus i am attaching copy from Cleveland tech section on end mills as the info is still good.
See page 6....pick the material and look at the recomended feed chip load for size of end mill, and get spindle rpm range.
Use the other info to adjust and easy calc to get you in the ball park.
I actauly did a spread sheet for the Atlas Mill based on available spindle speeds fly outs of info, and does all the calc's
( never use it ....easier to look at the tables ).
Carbide is great, but watch it as you can break them easier than say cobalt end mills. Backlash can kill one on a deep cut .
from the hobbiest FWIW, ;)
RICH
-
Just to add up to what Rich and Dave said about carbide end mills. Avoid hand spraying with carbide tools as the fast temperature drop may chip them.
Dan
-
HHS for that app I would use 500 rpm and feedrate of 10 IMP doc .050" then set FRO to 50% adjust from there. Lots of coolant if a avaliable. Monitor chip load and chip color. Even cuting with 1/4" bit not a problem IF your cut paramaters are correct.
(;-) TP