LinkBack URL
About LinkBacks
Sounds like a VF2 would be plenty big enough.Originally Posted by carson935
As far as drilling and taping why not just do a second and third setup instead of paying for the 5 axis trunion or a 2 right angle heads?
| | |
Total newbie need help with machine selection, I know very little about CNC machines!
We have a handful of die-cast parts that are currently machined for us on the outside. The machining consists taking up to a 26" diameter part and machining a bore and keyway in the center hub of that part. Next, I have to drill and tap two setscrew holes (1/4-20) on the side of the hub (the entire hub is about 3" in diameter), intersecting with the machined bore. The setscrews need to be 90 degrees apart from one another.
Anyway, we are considering bringing this process in-house so I flew into Chicago for the IMTS show last week to learn more about the CNC machines.
The best fit seems to be a VMC.
From what I've learned, we would use one tool to machine the bore, a second tool to pre-drill the keyway, a third to finish broach the keyway, and then a right angle head to drill the setscrew hole, spindle index that head to drill the other setscrew hole, and finally switch to second right angle head to do the same process but with a tap bit.
This solution would eliminate the need for 5-axis trunions or even indexing tables. It may also allow me to put more than one piece on the machine bed at a time so I could be doing 2 or more pieces per cycle.
The material is aluminum and I want to have a per/piece cycle time of approximately 2 minutes or under.
The machines I identified are the Haas VF3 or the Mori Seiki DuraVertical 1035 (I think thats the model number).
Here's my analysis so far:
Haas advantages -
1.) US made so better parts availability
2). Cheaper
3.) More versatile if I ever wanted to do other things (more cabinet area and more machining area).
4.) More popular, larger install base
Haas disadvantages -
1.) Debatable if the right angle heads can be used in the tool changer or if they would have to be picked up off the table
2.) Some people (remember I don't have any personal experience with this) claim Haas is closer to a "5 year" machine that would be junk after that time frame.
Mori advantages -
1.) Faster spindle speed standard (although I don't know that I need it)
2.) Better reputation
3.) Tools are kept out of the work area (Haas only does this if I upgrade to a side changer which I don't need).
Mori disadvantages -
1.) Foreign made - Could I be in a situation where I'm waiting for parts from Japan?
2.) More expensive.
3.) Unclear if service vans are as well stocked
4.) not as large of a machining area
In the end, I'm not sure I'm as concerned about the cost. If the more expensive machine is truly worth it, it's easy to cost justify. I want a machine that someone (someone contracted - not me!) can setup the programs and the darn thing will just work. And keep working!
The accuracy of the setscrew holes aren't critical but the location and perpendicularity of the bore is. I don't want something that can't hold my tolerance 3-5 years down the road.
Also, because this is a production machine, I need to know I can get back up and running quickly if the machines does go down.
I'm leaning Haas just because of the US and versatility advantages, but I'm torn. Any feedback the experienced users could give me - one way or another - would be greatly appreciated!!!!
Sounds like a VF2 would be plenty big enough.
As far as drilling and taping why not just do a second and third setup instead of paying for the 5 axis trunion or a 2 right angle heads?
The VF2 would be big enough. For the price difference though, I figured I'd go with the 3 just for the larger work surface in case I wanted to setup more items on the bed at once.
A multi-step fixture would work, but I'm concerned about my 2 minute cycle time if I spend too much time moving between fixtures.
My opinion is the machine time is only part of the total cycle time. How will this 26" part be fixtured? An operator using an air hose to blow off the coolant and chips, then removing the finished part and loading the next part will likely take nearly two minutes per part without including the chip making. That's a big part to blow off every cycle. How many parts are needed per shift? Per week?
The industry has clearly demonstrated the Mori is the more capable machine. However, the performance advantage is not automatic. The Mori can take advantage of better tooling and programming but, like a high performance car, crippling it with a mediocre driver (no offense intended) and cheap tires will prevent it from performing as well as it can. For your application, tool change time is going to be important.
Service varies region. Ask other shops in your area what their experiences are with the local dealers and the factories. If the local dealer is a schmoo, the brand won't matter.
Since you're starting off with castings, I think one absolutely mandatory option is the probing package. This will allow you to automate correcting for any casting flaws and how they relate to your fixturing. The downside is that, with the parts you are making, you will have to make a very accurate subplate for the tool probe so you can remove it once your tools are set to allow for the parts to take up the entire table. Or, get a bigger machine.
Speaking of fixturing, you say the parts are as large as 26" in diameter. The VF-3 only has a 48" x 18" table. Since you are machining the center of the part, and assuming you have two parts on the table at once, I don't see how you're going to hang on to these things unless you are using air or hydraulic operated clamping systems that hang off the table in both directions. A picture of the part would help.
One thing you made no mention of is quantity. This will make a huge difference in how you go about these parts.
You also didn't say anything about the tolerances of the ID bore, and how thick the part is. You say perpindicularity is critical, which to me says you need to bore it, not interpolate it with an endmill. So, what you're really looking at is:
T25 - Probe
T1 - Endmill to rough bore
T2 - Boring head to finish bore
T3 - Double angle cutter to chamfer top/bottom of bore
T4 - Right angle with tap drill
T5 - Right angle with chamfer tool (does both ID and OD of hub for setscrew holes
T6 - Right angle with tap
Aint no way in hell that's a 2 minute cycle. You say you don't want the sidemount toolchanger, but that only puts you further from your cycle time goal. Check out some videos on youtube of the two style toolchangers running and make your own decision.
EDIT:No offense intended here, but you may want to think very seriously about hiring an experienced CNC mill guy to come in, take a look at your parts and design a manufacturing solution for you. I think you may be unaware of a lot of little things that are going to jump up and bite you. Buying a machine for a job shop is one thing, but buying a machine for a specific family of production parts when you allready have a (unrealistic, IMO) cycle time goal is a whole nother animal.Total newbie need help with machine selection, I know very little about CNC machines!
No offense taken! Like I said, I'm very new to this and I appreciate any and all feedback.
Let me answer a few questions that have been asked:
1.) In reference the part, or multiples for that matter, not fitting on the table. The part is not a full circle. I know I said it was 26" in diameter but I unintentionally misled people with that. It's more like a 4" thick lawn mower blade that is 26" long, but only 6" wide.
2.) Bore tolerance is .6251-.6258
3.) Perpendicularity tolerance is .007
4.) Part quantity is 150-200 per shift (currently 1) every day.
5.) The reason I prefer not doing a straight bore is I need a very smooth surface so I would also have to ream then. Also, we have done this in the past and always ended up with some degree of taper which is not ideal. Last but not least, wouldn't I have to be more concerned with tool wear and it's effect on the tolerance in a bore scenario?
6.) Production method - The right angle head scenario is how the current outside vendor is producing these. He has confirmed to us that his machine cycle time is just under two minutes. Granted, he is using an index table, but in talking to the vendors at IMTS, they said we should be able to us spindle indexing and get the same result for our application.
7.) Good point about the probe system. I didn't have that listed but I am configuring the machine with that options.
8.) Tool changer - good point here as well. I wasn't going to upgrade to the side tool changer because I didn't need that many tools. However, when looking at the specs again, I see that the tool change from an umbrella is almost three times slower than the side tool changer, I will go with the side tool changer just for the faster tool changes.
My opinion, for what it is worth, is that you should stick with your supplier if you are getting these done at sub two minutes per cycle.
But I do have a question based on this ....then a right angle head to drill the setscrew hole, spindle index that head to drill the other setscrew hole.......
Can anyone explain how you 'spindle index' a right angle head when it is fixed in location by a dowel pin that locates in a block bolted to the spindle nose?
An open mind is a virtue...so long as all the common sense has not leaked out.
Yeah that probably won't work, you'll need another angle head. Shouldn't be a problem although the added cost for those things brings a tear to my eye
It sounds like you're in a position where you totally absolutely need to make these things on your own instead of outsourcing them, and the cost isn't much of a prohibition. When I've been in those places in the past I find it's useful to figure out where the actual cutoff lies in terms of machine cost. I mean, there's always a ceiling somewhere, and for me it's always where the bottleneck gets placed. If you have an unlimited budget then the answer is simple, buy one machine for each operation
Anyway I'm not sure how much time you spent looking at horizontal mills, but those are always an option for multi-side machining, especially large parts that are [often] not too difficult to mount on a rotating tombstone inside a horizontal mill. Often you need longer tools to reach around the side of the part, but that's definitely where horizontals shine. The machines are a bit more expensive but it's easy to configure them with pallet changers and the like, great for high production.
Not sure of your exact part shape but you could look at the work envelopes they give you and see if anything fits.
1. Please provide the specs for the right-angle head, to advise on tool change capability.
2. There are many Haas machines in use today that are 20+ years old.
The right angle head I was looking at was from Koma Precision and is the Alberti T90cn-0,5C.
It was selected because of it's narrow neck and it's ability to get at the center hub of my piece (there are clearance issues getting at the hub).
The Haas rep at the show said we could use spindle indexing. Is he wrong (I wonder if wasn't thinking about right angle head stop blocks when he said that)?
If spindle indexing isn't an option, would you recommend another set of right angle heads or would you go with a rotary indexer (taking cost out of the equation for the moment)?
You aren't far from the mark. I need to be able to control my own destiny and with my current vendor having capacity issues with existing volume, I'm thinking it's time to control my own fate.Yeah that probably won't work, you'll need another angle head. Shouldn't be a problem although the added cost for those things brings a tear to my eye
It sounds like you're in a position where you totally absolutely need to make these things on your own instead of outsourcing them, and the cost isn't much of a prohibition. When I've been in those places in the past I find it's useful to figure out where the actual cutoff lies in terms of machine cost. I mean, there's always a ceiling somewhere, and for me it's always where the bottleneck gets placed. If you have an unlimited budget then the answer is simple, buy one machine for each operation
The ROI for bringing the operation in-house is very compelling (less than a year payback) so I'm not overly concerned about the machine/tool costs as long as I'm getting value for what I pay for.
For drilling and tapping that cross hole, personally I would use a cheap drill press and make a dedicated fixture to do the cross hole. You can use a Tapmatic head with a drill and tap bit, like one of these, http://www1.mscdirect.com/CGI/NNPDFF...0&PMT4TP=*LTIP . This would save the expense of a right angle head on the CNC machine. You could make a manufacturing cell and have the operator load the part in this fixture and drill and tap the hole in 1 shot while another part is on the CNC machine. At least this is what I would do in your situation.
Good luck.
Posting Permissions
| | |
