Can this be cut on haas with rotary??

[Roger]

Can this part be machined on a Haas VF-5 mill, with rotary using Mastercam mill level 3? Or do I need muti-axis? If so, what tool path would you use?

 

Thanks

[JoshC]

it really depends on the toolpath strategy you choose. without multiaxis you limited to using axis substitution and from looking at that geometry it would be difficult in my opinion to get axis substitution to accomplish that. Alternatively you could do more of the 3+2 type of programming where you position the 4th, surface as much as you can and repeat. This process you could do however you probably going to have a far greater run time than if you were using multi-axis paths, so in my opinion you would need to weigh the cost of the extra run time and programming time required in comparison to the price of the multiaxis package. if you plan on running lots of these or have intentions for similar parts in the future i would say contact your re-seller and get yourself the multi-axis paths, if not 3+2 type of work should get you by. Good luck bud.

[Roger]

Thanks, Josh

 

I'm wondering if I could get the muti-axis for X6, without updating the rest of my seat. This is my personal seat of MC, which I've had sense V7, and really don't want the cost of updating everything. (Lathe, Solids, Mill level 3). I'm no longer on maintenance.

[djstedman]

Cool looking piece, Given the almost non existent internal corner radius where the two sides meet in the middle I would say its going to be a challenge to cut it at all.. (if you have to hold such a small internal rad)

 

I think if I were to do this.. I would attempt to cut one tooth space by cutting it at about 1 or 2 rotational positions.. to make sure there was proper clearance to avoid gouging any undercut locations..

 

It looks like with the right rotation it could probably be done in one shot though.. so long as your cutting the tooth space and not a tooth..

 

If you have to use more than one path to get at it all, the hardest part would be coming up with clean toolpaths.. making new surfaces that only include the parts to be cut from each position would probably be the easiest way to accomplish that.

 

Once that was complete I would do a transform toolpath to rotate the original paths however many times to make the proper number of teeth.

 

I could be wrong but I don't think there is any real reason to believe that a multiaxis path would get the part cut a lot quicker. Now don't get me wrong.. it would be a whole lot cooler to watch it run as a cool multiaxis path, I am just not convinced its strictly necessary to produce the part..

[Newbeeee™]

Am I missing something??? but bottom left hand view where the flanks 'raise' and meet in the middle, there appears to be no fillet rad.

So how would you cut that?

[Newbeeee™]

DJ beat me to it - me tooooo slow typing

[Joe788]

There's no undercuts, so it should be no problem with Mill Level 3 if you just want to 3+2 it. Program one groove with whichever 3D rough and finish strategy tickles your fancy, transform>rotate the toolpath 8 times, and call it a day.

 

Depending on the material and what options your machine has, you'll most likely get better results with 3+2 anyways.

 

 

(Edit: this is assuming there is some allowable corner radius in the spot others already pointed out)

[BenK]

There's no undercuts, so it should be no problem with Mill Level 3 if you just want to 3+2 it. Program one groove with whichever 3D rough and finish strategy tickles your fancy, transform>rotate the toolpath 8 times, and call it a day.

 

Depending on the material and what options your machine has, you'll most likely get better results with 3+2 anyways.

 

 

(Edit: this is assuming there is some allowable corner radius in the spot others already pointed out)

 

+1

[Roger]

The sample part has radius in the corners. The mill is a new Haas VF-5 with full rotary. (HRT 210, as of now not been used). This is a prototype part. The sample is out of aluminum, they might change that to brass, nylon, or keep it aluminum. I just need to let the customer know if we can do it given our equipment.

 

We're a new machine shop, (4 months). I've been a machinist for 34 years, the last 16 years has been CNC programming, machining. I've did some rotary work before, just positioning, rotating, and some horizontal mill work. So, if I can do this job here, I'll be asking for A LOT OF HELP HERE ON THE FORUM.

 

Thanks for all the replies, please keep them coming!

[crazy^millman]

Roger, yes. The other guys have pretty much pointed you in the right direction. I just completed a 11 blade impeller with no 5 axis toolpath what so ever. The machine I was programming it for is having issues doing full 5 axis and had to do it in 3+2. Probably double or triple the work, but got it done. That is the difference we figure what we need to get the job done with what we got. Some like to just complain how much Mastercam sucks others of us do what needs to be done to get the job done. You sound like you are on the right track and if you can have Full Profile tool Made, might think about Roll Die or Even Axis Sub so you could cut in one operation to finish to ensure you make the shape 100% to what you are looking for. With Surface machining you will get what you see on the sample part, with a full profile tool yes you will have a big radius to worry about in the corner, but if you are making the mating parts then everything would match and all would be okay. Just a different way to think about it is all. Let us know how it turns out look like fun and please some of us like to help others.

 

My ignorance to help others is strong so will keep being the simple person I am.

[Thee Rickster ™]

My ignorance to help others is strong so will keep being the simple person I am.

 

If you think you are simple, you are CRAZY!....