fadal 5axis A axis feedrates

[octhesax]

my shop has a Fadal 4020-5th axis (XYZ A&B axis). The part is made out of t700s graphite composit,.300 thick and I'm using a curve 5axis toolpath set to 4th axis output.

The part shape has some twist to it that need to stay perpendicular to the top surface. I can get it to do the the path(in mastercam)and it looks good. I have posted to machine and watched it run(cutting air),looks ok. my problem is the feedrate that the post outputs. using f300(for example) it goes fast in the straightaways. when there is a simultanious XYZA move, it slows down. so it speeds up and slows down as it rotates.

can anyone help me figure out how to keep a constant feed throughout the entire cut.

thanks guys, oscar

[Jim Whipple]

Just a thought...

Do you have the HSM box checked in the Job Setup page?

 

I think that's the only thing that will get you variable feedrates.

HTH

Jim

 

[ 12-12-2002, 10:14 AM: Message edited by: Jim Whipple ]

[Claytonic]

You Could try and use create arc out put in xy, zx ,zy found under total tolerance button. Depending on your setting you can get mostly arc's. Iv never tried it on a 5 axis machine ??? hope this helps.

[octhesax]

"Do you have the HSM box xhexked in the Job Setup page?"

 

HI JIM, I'm not sure what you mean by HSM box. I don't see any box with that description.

Im using version 8.1.1 . maybe thats the problem?

[Jim Whipple]

Sorry... It's the adjust feed on arc move button

 

And I'm still way back there at V8.1.1 too

Jim

[octhesax]

HI JIM , NO i DIDNT HAVE THAT TOGGLED. I'LL TRY IT, POST IT SEE WHAT THAT LOOKS LIKE, I'M ALSO THINKING I NEED TO TAKE A LOOK AT THE POST ITSELF. WE HAVE NEVER TRIED ANYTHING LIKE THIS BEFORE(CURVE 5 AXIS TOOLPATHS) SO OUR POST MAY NOT BE UP TO SNUFF.

THANKS,

OSCAR

[cadcam]

As it starts to move in all axis being X,Z,B & C at the same time the post turns this in to inverse time were it is limited by the axis it self.

 

The rotary table or gimble setup has a feed rate limit on how fast it can turn compared to the faster speed of the say X, Y & Z being straight leaner moves.

[octhesax]

HI Jay/ aka CadCam,

You have the best explenation yet:) can you explain to me how then I would go about fixing this? Do you think it is the way our post is set-up or do you think it is in the FADAL parmeters itself. I'm not too clear on how that inverse time works. can you point me in the right direction. Is there a certain formula to use to get all axis to move at a constant feed rate? Is there a setting in MASTERCAM? I noticed it spit out G93 codes. according to the FADAL manual explanation, it is for controls that did not interpolate XA or YA moves. maybe we dont need it? I looked in the post and this is how it was set: "use_frinv : 1 #Use Inverse Time Feedrates in 4 Axis, (0 = no, 1 = yes)#WAS 0" I changed it to 1 before I posted thinking it might fix things. but I think I tried it before(a couple weeks ago) I made the change in the post and got the same results. I would really apreciate any help can offer.

just for kiks i included a sample of what my test program looks like. I striped all the feeds except for the first one. the post spit out feeds on every line that were the same. except for a few different ones. thanks again Jay, err' I mean CADCAM.

thanks, oscar

[Trevor Bailey]

You should probably look at the info that came with your added drive and make sure that you can safely increase the feedrate. It may be set to optimal cut feed already.

[Guest CNC Apps Guy 1]

Here's the other thing, as you add axes in simultaneous motion, you're placing a larger demand on the processor that controls the machine, so you may be maxxing out. Ever run a surface toolpath that you programmed at say.... 400IPM, and it only gets up to 250IPM or 300IPM ??? Same principal is in effect.

 

Something to think about.....

[cadcam]

the G93 that I remeber is were it changes to inverse time if I am correct when this code comes up just as it is going to do the other axis at the same time?

[Trevor Bailey]

You said a mouthful there James. I was at the Fadal factory yesterday doing cut test on different machines. What a joke!!!! The best machine I saw for what I need was their Performance series with a Seimens control. For $100,000 plus, it cut great. HOWEVER, I can purchase a VF3 Haas for $40,000 less that cuts just as good with the feeds/speeds I need.

 

Once again, what a joke.

[cadcam]

Trevor you were down nere me and did not call.

What a pal.

[cadcam]

octhesax after viewing your file this i would say that your hold up is the inverse time in the "A" axis.

 

there are only X,Y,Z & A movements.

I had gone thru this before and trying to remeber what to do.

 

James any thouhts at this time? the post is using the inverse time due to the added A's in the movments.

Can we just turn off the the Inverse it is marked on.

[octhesax]

HI CADCAM,

I'm just I made change in post and right now I'm just waition to get on the machine as it is being used at this time. Hopefuly you can remember how you got around to fixing your problem before.

thanks, oscar

[Trevor Bailey]

My bad Jay. I was with the owners out shopping and had a one track mind.

[Guest CNC Apps Guy 1]

Some machines require Inverse Time and some require Degrees Per Minute and some will take either. Inverse time adjusts the feedrate accorting to the center of rotation's relationship to the pivot point (at least this is how it was explained to me), this is why you see feedrates on almost every line.

 

The only thing I really have to chime in on is what I said before. It may be that the Control can only process blocks so fast and the more information contained on a block, the longer it takes to process it, also, if the moves are very small and lots of them, this bogs things down as well.

 

Hope that helps in understanding the process. Ya know, it's not just about feed rates. It so much more than that.

 

JM2C

[octhesax]

thanks james for the input, Its starting to make sense. just gota play with it till I get it right I guess.

p.s. do you really look like like the picure I chuckle every time I see it(nno ofense) oscar

[cadcam]

quote:

---

p.s. do you really look like like the picure I chuckle every time I see it(nno ofense) oscar

---

All my students asked the same thing.

 

Don't worry James I told them you don't really wear the hat.ROFL

[Guest CNC Apps Guy 1]

 

Yeah, I don't usually wear that hat. I usually wear my USC hat!!!! LOL!!!

 

I don't look like that. It was a picture I found on the internet somewhere and I knew I'd have an use for it someday so I grabbed it.

 

I just met with gcode a little while ago and gave him a tour of the school. He can attest to the fact I am much less hansome than the picture!

[Jack Mitchell]

Octhesax,

 

The axis of all will sync to the slowest and adjust accordingly, Mastercam will not overcome the laws of physics nor will the Fadal, manually programming the multiple axis will prove this.

 

The rotary axis probably revolves at about 20% of the feedrate that you were expecting, multiple processors will certainly do the math very quickly; however, this is a mechanical problem brought about by introducing one or more rotary axis to the mix.

 

G94 vs G95 matters not; play around with the feeds and you will learn a little more.

 

A scientific approach or explanation is required here, unfortunately - we are a hindered breed when it comes to explaining some things.

 

Regards, Jack

[Trevor Bailey]

octhesax,

 

As I mentioned in my earlier post and now, also Jack has mentioned, I think you are dealing with machine limitations. You may want to contact Don Ackerman. He used to run that machine if I remember correctly. That is if Kelly will let you. By the way, tell her I said hello.

[octhesax]

HI TREVOR, KELLY SAYS HI BACK. I KNOW DON ACKERMAN VERY WELL(WORKED WITH HIM FOR 5YRS), IN FACT I TOOK OVER HIS POSITION. I KNOW THAT THIS IS BEYOND HIS KNOWLEDGE(NOT A PUT DOWN,I JUST KNOW THE THE GUY ITS JUST THAT THE PROBLEM IS IN THE POST PROCCESOR. THERE WAS A FEEDRATE LIMIT IE="maxfrdeg : 300 #Limit for feed in deg/min" #WAS SET TO 150. SO I JUST NEED TO MESS WITH IT AND TWEEK IT. WE DONT HAVE POST THAT WORKS RIGHT OFF THE BAT. AS WE HAVE NEVER DONE ANYTHING LIKE THIS BEFORE...BUT THERE IS A FIRST TIME FOR EVERYTHING. WISH ME LUCK AND THANKS FOR ANY HELP GUYS. P.S SORRY FOR THE CAPS

OSCAR

[Trevor Bailey]

Have you checked with Charles. If I recall, we worked on a 5ax post for a Fadal before a while back.

[Dave Jablonski]

Inverse feed is usually required when machining 4 and 5 axis parts. Most post processors do the math and output the feeds correctly. Sometimes the only way to adjust those feeds is to edit the toolpath.