5 ax NOOB

[HEED]

So, our shop is getting our new 5ax tilt rotary table within the week (scheduled) so maybe by the end of summer it will finally be in ... What do I need to know about programming etc. I have the in house solutions book on 4th and 5th programming, but as well as the MCX samples they all seem to be kind of BS parts, not really real world examples and it's just like - click this do that , no explainations of what you are doing to it... As far as I know (very little) about the programming you actually draw and machine off of c/l does that mean that you set up then program ? The local MC dealer is kind of one of those "too busy to help " types, is there any good online training, how did you all learn the ropes? I am pretty sure the company would fly an instructor in, or send us to training somewhere... Thanks

[Guest CNC Apps Guy 1]

quote:

---

...they all seem to be kind of BS parts, not really real world examples...

---

See, that's precisely the wrong attitude to have. Just about evry part demo I've ever seen has real world application. So whjat if they parts are simple and don't "look like a real part". You hve to be able to apply the principles of what you learn on one type of part to another type of part. Us 5-Ax guys were't born programming impellars and blisks. Besides... are YOU going to contribute YOUR or YOUR CUSTOMERS parts to whomever as demo parts??? Guessng not. Sorry to blast you but to learn anything, you've got to have the right attitude. I taught Mastercam for a few years and a number of students had a tougher time learning the concepts on a complex "real world" part. It all comes down to do you want to apply what you learn...

 

quote:

---

...no explainations of what you are doing to it...

---

I'll give you this one. The resources do need to do a better job of explaining the "why". That's a legit gripe.

 

quote:

---

...is there any good online training...

---

Streaming Teacher is about the best I've heard of.

 

quote:

---

...how did you all learn the ropes/

---

Took a few semesters at te local Comunity College, pad close attention to those around me that were better than I was (nearly everyone in the beginning), asked lots of questions, got a lot of breaks. That's it in a nutshell.

 

CNC Software does do training at their facility if you want to get on a plane...

 

HTH

[HEED]

I know it's a bad attitude to have about the training but I think I got off on the wrong foot with the whole click here do this - I wish it explained it a little better but as I pick it up I am sure that it will all start to make sense. And I can understand how they would want to simplify it so that it's just one principle at a time I took the 3ax. class at the local community college, but as the area is more geared to the 3ax and 4ax indexer, there are a few local shops running 5ax, and I know a couple 5x programmers (few and far between) but I wouldnt want my guys showing the competetion how to make our parts , So I am going to respect boundries and get some education another way. I think that the best thing would be to bring a trainer to the facility is that an acceptable practice ? That way training would / could be more specific to our needs.

[Guest CNC Apps Guy 1]

quote:

---

...I wish it explained it a little better...

---

As do most people that use/have used the training materials. In-House is very responsive to customer suggestions. If you've got some suggestions, I'm sure they are all ears. It's part of how they make money and they want to give their customers the best possible product.

 

quote:

---

...they would want to simplify it...

---

Yeah, that's the key to retaining what you've learned. Take it in small enough bites that you never get full, whereas if you got the whole enchilada, we'd be quickly overwhelmed.

 

quote:

---

... I think that the best thing would be to bring a trainer to the facility is that an acceptable practice?

---

I belive it can be a good thing. If your company will allow you (and your group) to be trained without interruption, than often times, the trainer can show you things specific to your pats wheich is often times helpful. The trainer can pick out certain features to show principles and explain the different approaches. One of th boggest part to doing 5-Axis is approach; "... how exactly do you want to cut it?..." Then you learn about the different toolpaths and what they make the tool do.

 

Training at your facility can be on the expensive side but the 4-5 placed that I know of that sprung for it said it was well worth it.

[HEED]

The company that I work for is fairly decent sized (2 mil. + a month ) out of our facilty alone, plus, china, switzerland, and all over the U.S., it's just frustrating that they never want to spend any to make product better / faster / more efficently etc. The 5th Tilt/ Rotary was a HUGE leap for us. I think that in house training would be awesome, but you did bring up a massively valid point with the no interruption. I dont think that would ever happen. Maybe the best thing is to take it in small bites, and work with the local MC dealer when I need programming help. I was pretty excited when the order first went off, but as it gets closer to installation I am getting more nervous about it, but I think if I take it as an indexer, then work into full 5 it will be a lot more smooth of a transition for my brain to wrap around.

[Guest CNC Apps Guy 1]

The majority of the stuff out there is 3+2, not 5 Axis simultaneous...

 

The more axes the fewer the limitations on what you can do. You maye have t do some thinking but it allows you to accomplish more in 1 clamping.

[Zoober]

quote:

---

...how did you all learn the ropes/

---

1. fetch coffee if not sweeping

 

2. "grab this box of files, and make this square pc of 17-4 into a round (within .01) ball"

 

3. work 3rd - or whatever worst shift is with very little supervision, reading machine programming and operation manuals during cycle times, but only AFTER parts are deburred.

 

4. get a demo version of your cam system and work many hours (no pay, of course) learning how to make parts.

 

5. be super nice to the best guys in the shop (coffee works well). Ask them as many questions as they are willing to answer

 

Repeat #s 1~5 as often as needed, for 10 years minimum.

 

Piece o' cake. HTH!

[produca2]

quote:

---

Took a few semesters at te local Comunity College

---

CNC Apps guy... what community colege did you go to that taught 5 axis? I live in So. Cal and would be interested in checking that out.

[Racerje]

Well I feel your pain Heed, not sure what the manuals you are reading has to say as i am learning 5 axis on the fly. The thing that took me a while to get used to is using C/L of part for your WCS and then changing veiws and planes so that you are looking at the part from the spindle, complex parts take alot of veiws and getting MC to get to those views can be frustrating (at least for me) at times.

I have only been using 2 and 3d toolpaths the 5 axis confuses me and I have only been doing the programming here for 1 month or so. we have the 5 axis option but we are so buried on programs that I dont want to change what I am doing so I can keep the machines running.

I work nights and read the Forums alot it really helps got some real good info from the great people in this forum

[Guest CNC Apps Guy 1]

quote:

---

...what community colege did you go to that taught 5 axis?...

---

I didn;t learn 5-Axis at the community college, just the bare bones basics, but I went to Mt. San Antonio College. While I taught Mastercam at the NTMA in Ontario I taught a few Advanced Mastercam Classes and we covered 5-Axis, BASIC post Processors, Solid Modeling, and a few other things. Funny thing about working with posts, EVERYBODY wants to do it... until they learn about it. I think I scared more guys off than turned them onto it... I did my job ... If you're scared of Post Editing, you SHOULD NOT be doing it.

[67 Yankee]

Some pointers to help you get going...

1) Program your parts in incremental mode. This will allow you to translate the part after programming. If you ever run into a clearance problem, or have to recut your fixture for some reason, or if everything doesn't fall into place quite as planned, being able to reposition your part is massively helpful.

 

2) pick one WCS and stick with it. I don't know about all trunion machines, but ours will tolerate only one part origin, and that is at the intersection of the A and B axis centers of rotation. From what you said, it sounds like yours is the same. I usually move my model around and orient it for best use of the TOP WCS/CPLANE/TPLANE and then program the entire part in the TOP work coordinate system. Use your TPLANEs to see and work on the non-TOP sides of your part.

 

3) Use circles to construct your GVEIWS. When you want to look at your part normal to a feature, you can pick GVIEW by entity but you will usually only have a few options concerning the orientation of the part in the new view. If you use the part geometry to construct a circle on three points, you can pick the circle as your GVIEW entity and you will have eight available orientations to set your new workplane. You can also use your mouse to rotate your viewpoint of the part to whatever you like and simply save the current graphics view. I like to do that when I have deep vertical fillets on a part and need to clean them our with a small ball end mill.

 

4) No doubt you'd like to see what's going on while the part is cutting, but it's safer to allow your part to tilt away from you where you can't see it behind the trunion. (My boss used to ask "can't you cut that out here where we can watch?") You can get a nasty crash that way and you won't see it coming if you're watching the tool. (No, I didn't have to crash it to learn! lol)

 

Simple stuff, but they may help you get on track with a bit of understanding. I also used the books for 4 and 5 axis as well as lathe programming, and I had the same complaint about doing stuff without knowing why.

[Thee Starry™]

quote:

---

4. get a demo version of your cam system and work many hours (no pay, of course) learning how to make parts.

---

Yep... That is the best route, IMO. PRACTICE, PRACTICE, PRACTICE. Take every minute you can spare and work with MC. Try new things, read the help files, follow the examples and videos in MCX. And ask a-lot of questions of the people here, in your shop, your reseller, and even other shops. I have MCX2 on my laptop and I bring it home to work with every evening and all weekend long just to try new things and find better ways of doing it.

[HEED]

Thanks for the replies guys I am just writing back in between cycles here so I didn't catch them all but it seems like there is a lot of info. here I know that it's just going to take a lot of practice time and lots of long days / nights pulling hair out, then an epifany (sp?) hits. I have been doing a lot of surface paths and even getting into some kind of "advanced" 4th stuff (MCX posting rotary moves for me ) so changing planes is not a biggie. I was thinking about it last night though... is running g54/55/56 for different orientations a(n) accepted practice for 5th indexing ? I dont see much indeding other than on the B , so lets say the first program would call g54 work the top side, sub would call g55 rotate a 90' b90' run, call sub g56 forate a90' b180' etc. ? Just thinking out loud... any input is appreciated. Thanks and I will reply again later tonight with more questions when I get a minute to read the replies. Keep Em' comin!

[67 Yankee]

You probably don't need to do any indexing, subprograms or fixture offset changes. (At least I've never had to do any of that.) Each operation will output the proper A and B values to orient the machine as you have programmed it. Leave all operations on G54 and let Mastercam do some of the thinking for you. Set your clearance planes well above the part to be safe at least until you get a feel for the part movement as it changes between programmed tool planes.

[crazy^millman]

There is a file on the FTP I did for someone called STARWORLD_5AXIS_CURVE_EXAMPLE.MCX see if that gives you some ideas about clearance and keeping tools safe as you do moves from one index to another.

 

HTH

[Racerje]

I have a question I have been programming 5 axis in 2 and 3d toolpaths is there any way to sim a rotates ? I was playing around with 5 axis programming and it shows the a axis rotating looks really cool. Too new to Mc and confusing to use 5 axis jus tgetting the hang og 2 and 3d toolpaths.

 

Thanks, Racer

[MIL-TFP-41]

quote:

---

so lets say the first program would call g54 work the top side, sub would call g55 rotate a 90' b90' run, call sub g56 forate a90' b180' etc. ? Just thinking out loud... any input is appreciated.

---

This approach "could" work, tho I think it could bite you in the a$$ if you were to accedentaly put in the wrong work offset. Your post will (should) output G54 A0 C0 at first(provided that is your first orientation) then when it comes time to reposition the tilt/rotary it should output A-90 C90 or whatever (note still using G54).

 

As for 5ax training in Utah....seat time is your best asset...but that could be said for anywhere.

[HEED]

quote:

---

5. be super nice to the best guys in the shop (coffee works well). Ask them as many questions as they are willing to answer

---

Well, that would be easy, other than there is really no one else in the shop that kows 5x (first one)

quote:

---

4) No doubt you'd like to see what's going on while the part is cutting, but it's safer to allow your part to tilt away from you where you can't see it behind the trunion. (My boss used to ask "can't you cut that out here where we can watch?") You can get a nasty crash that way and you won't see it coming if you're watching the tool. (No, I didn't have to crash it to learn! lol)

---

Why is it safer to tilt away from operator, I would think it would be better to tilt toward operator so you can see what is going on ? Haha, James you are one of the few guys I know of around here that I mentioned in one of the above posts about not bugging... Funny stuff that you would end up on here helping anyhow ! When you program for the indexer to go to let's say "front plane" or any other index , do you reset the t/p or not ? And if you have a(n) index at a wierd angle (33.25 for ex.) do you create a new plane at 33.25' ?

[67 Yankee]

With the part tilted toward you, the trunion can hit the bottom of the head assembly when the tool is reaching down into the part. With the part rotated away from you, that can't happen.

[HEED]

ahhhhhh..... I see now... That could pose a problem. It's so simple I should have thought of that. I guess it's like machining on the backside on a horizontal then. Ron, I pulled up your FTP file, and am I EVER confused. WTF is going on with the point toolpaths ? They dont change the tool plane are they just there for clearance ?

[Zoober]

quote:

---

And if you have a(n) index at a wierd angle (33.25 for ex.) do you create a new plane at 33.25' ?

---

Generally, if you need to create a view at say 33.25, it is because you need to machine a feature in that vector. Therefore, there should be some geometry normal to that vector. You can create a view by solid face, or geometry. What I often do is go to top, then rotate my GView to the desired vector, and then use "name and save the current graphics view".

[HEED]

ok that works for the view but do you have to change the active tplane to reflect the 33.25' or do you stay in top tplane and let the geometry (solid face , etc.) do the work ? I guess the question is would you need to create a new tplane at the funky angle or does the geo figure it out for you?

[Zoober]

Depends........

If you are doing 3+2, then change CT planes to that new view. That is what triggers the tilt/rotate. If you are doing full 5ax, then leave at WCS, and the cycle will do the work.

Hope that makes sense...

[HEED]

Totally it makes sense just like the front top bottom back that I do when I index "a" around to do work on all sides. I guess you would just use every plane except bottom then ?

[Zoober]

pretty much. You will use whatever views you need, including creating non-standard, to achieve your normals. Granted, you can only use views that the machine can physically move to....