5 axis post

[steve f]

Hi, post guru's.

 

I'm in the process of modifying the MPGEN5X_FANUC.pst file for a customer's five axis router and acctually have working code being output right now. I have two questions some of you out there may be able/willing to help me with and any help would be greatly appreciated. I'm getting less than desirable results by using the job setup stock values (plus an increment) to set the axis travel limits that are used to calculate retracts between operations. I like using the limits variables (up_x_lin_lim, etc..) but would also like to be able to write the limits values calculated from stock dimensions yet keep a lower z limit (lw_z_lin_lim) of 0.0, and an upper z limit (up_z_lin_lim) of 6.0 or greater.

 

I've tried creating a formula but get errors in the post saying something to the effect that the result of a global formula cannot be used in a postline formula.

 

I'd also like to find a way to change -0. rotary ouptut to a value of -360. The rotary axes on this machine don't recognize minus (ccw) rotation direction if the output is to zero degrees and it creates a situation where the machine is running onto it's rotary limits even though the windup calculations in the post are working fine.

 

Anybody?

 

thanks in advance,

 

steve

[crazy^millman]

Look here: Good freaking luck!!!!!!!!!!!!!!!!!!!

 

You sir have hit the holy grail of questions.

 

The PSB is the key and guess what you can not and will not ever have access to it. I say this at risk to something I would like to do and that is be a Beta tester but oh well. People who spend the money for 5 axis machines are automaticly at the mercy of this sitution with any software company out there. I think we should be able to adjust a post that is suppose to be free and customizable but good luck. The pmx0 and other parts that are needed for this control well are out of reach to you and me. I wish I had the time but who does to delevlope a good fully working 5 axis post I would give it away not to xxxx off dealers but to make this profession go and be able to grow where it needs. We have all been there and it sucks trying to get the people with the money to do the right thing almost always they never do. Who is stuck picking up the pieces the little guys who work their fingers to the bone and try to live a honest life and provide for their familes. I don't want to rob any one by having access the the PSB of a free post I just want to be able to do my job and do it well. Yeah in this day and time that seems to be to much to ask when it goes against the bottom line. Call me a dreamer but still believe you help me I help you and those who know me know it is not about the bottom line with me.

[DavidB]

Well said crazy.Been trying to get a 5-axis post from reseller for a year and who does the Boss take it out on????

True what you say alot of poeple buy a 5-axis machine and then realise just how important a post is to the equasion.

There are just so many variables with 5 axis machines and what each operater would like.

 

Heres to the future

[steve f]

thanks for the replies. I guess I'll have to just keep hacking away until I come up with something resembling success.

 

steve

[Andris Skulte]

Millman^Crazy,

Simple question - what is a "PSB" (guessing something like source code?). Thanks!

 

Andris

[Guest CNC Apps Guy 1]

Section of Post coverted to Binary for protection reasons.

[MIL-TFP-41]

IMHO...mastercam is seriously shooting themselves in the foot by not offering a decent 5axis post. As a matter of fact, they are way behind their competition...both Surfcam & Delcam have FAR FAR superiour 5 axis support.

 

Mastercam DOES NOT even process gouges when using a swarf toolpath.

 

its amazing...I fought & fought a part, always came up with gouges till I talked someone into giving me code from Surfcam...same geometry, far different results.

[chip]

OUCH!

[MichaelJ]

did he now that was his 10 post look out

[MIL-TFP-41]

To expand on my post above....

 

I do not believe that gouge processing is a post problem....rather it is a Mastercam problem. Mastercam DOES process gouges when using a curve 5ax toolpath. Look at the menu's very closely...on the swarf 5ax they have something called "floor gouge processing"....on curve 5ax it is renamed to "gouge processing".

 

5 axis machining is becoming commonplace. Mastercam has always excelled in 3 axis machining...they are being left behind in 5axis support.

 

quote:

---

originally posted by MichaelJ

did he now that was his 10 post look out

---

post count = knowlege?

[gcode]

code:

---

 post count = knowlege 

---

No, new members who sign up and ask for a free post or rant about how crummy Mastercam is

get imunity for 10 posts before the flame throwers come out.

 

I make my living doing 5x work with Mastercam.

It does a very good job if you know what you are doing.

 

another cute computer saying...

Garbage in Garbage out.... even with Mastercam

[crazy^millman]

Well to claify my stand on 5 axis and Mastercam I will say this. Mastercam will do any thing on a fully articulating head 5 axis router that I can dream up and I am not called Crazy for no reason. The probelm most people have with the swarf toolpath is not using it for it what it is designed to do and usign the proper controls for sync the head movement to do what you want it to. I would never use swarf to do a inside corner or the bottom mating surface that was complex. If I was making side wall with no bottom or doing trimming operations then this to me would be the perfect toolpath to do so. Let us take this toolpath an examine what it does. It take a bottom chain and a top chain and then cuts that to your liking. If the control for that make thes tool go into a surface you do not want then how can Mastercam being doing the wrong thing when that is what you told it to do. I have used all of the 5 axis toolpaths as well as all the 3 axis toolpaths in 100's different c-planes the limits of Mastercam and 5 axis work is only limited by your imagination.

 

My complaint has and will always be the things I need to do my job and do it right are locked up when it comes to the post, but I still make good parts just alot harder to do so is all. This has not a thing to do with Mastercam doing good 5 axis work and its ability to do so. I have seen the other software and to say Mastercam is lagging far behind tells me you need to learn more about Mastercam before making such a statement. I ask you put up this file that caused this remark:

quote:

---

its amazing...I fought & fought a part, always came up with gouges till I talked someone into giving me code from Surfcam...same geometry, far different results.

---

and let others see this and see if we have a better solution and come up with this major difference you are talking about. Now if you are choosing the wrong toolpath then I guess you might need to rethink your stance on how terrible Mastercam is for 5 axis work, but since I know you will not put it up might need to rethink such a opinion that you can not back up with something for others to see becuase I will be more than glad to send you some stuff that I promise will blow your mind.

 

Got my Flame suit on as I was typing this.

 

 

And I will tell you as I have told others that post count don't mean a freaking thing to me.

[MIL-TFP-41]

I never said that Mastercam was terrible, but it does need some improvement. Crappy???...no...perfect???...far from it.

 

that being said and in responce to Millman's post above, I am uploading a zip file named JMCSWARF.zip (in the MC9 folder)

 

inside the zip file I have the part, a .nc file, the post used and a .doc file that I hope explains what I "think" is happening.

[Guest CNC Apps Guy 1]

quote:

---

...I make my living doing 5x work with Mastercam. It does a very good job if you know what you are doing...

---

+1

 

Perfect? No, what is???

[Charles Davis]

A free 5-axis post? Wow. I know some other systems charge thousands, or tens of thousands, for a custom 5-axis post.

 

The "free" post is CNC's property, and it's thier right to lock out parts of it.

 

Of course, you could always contract with a company to write a truly custom 5-axis post for you. It might cost $5,000, but it would eliminate your issues and would still be a bargain over most other systems.

[Steve Biehl - Cimquest Inc]

Charles,

If I was to write a 5-axis post from scratch for someone, it would cost more than 5K for that one up development.

 

The MC posts are great places to start, and are very close for Fanuc generic.

[crazy^millman]

JMC I had no problem doing what you wanted with swarf 5 axis. I trimmed your control surface ot the chain you were using. My only question is why would you want to use a falt endmill in the raduis corner. I would think that you would want to use a ball endmill and in that case I would use a Flow5ax toolpath and then create myself some axis control line and would be good as gold. I would problay start my frist as 45 degree to that surface then around each arc have the head povit at a central poivit place and the 45 dgree from the next and so forth. I also hope you do not take this the wrong way but 3 axis is how I would apporach a part of this nature.

 

I put up CRAZYSWAFTTEST.ZIP take a look. If you are using a rotuer when is the last tiem you chekced to make sure your head was in line and not out of alignment. You might also look ot see that if you are usign a poivit distance that it is correct.

[MIL-TFP-41]

Millman,

Did you look at all the levels on that drawing? It could be done via 3 axis, but there are already alot of surfaces being generated and doing that particular area would add that much more time.

 

I used a flat endmill for an example only, the actual part was cut with a ball.

 

The machine that it was run on is a maching center with a tilt/rotary table....A Matsuura Vmax-800 5axis to be exact. Siemens 840DI controller.

 

were you able to post out a program where the c axis did not reverse itself? These are the causes of the gouges on the walls.

[steve f]

After alot of work on the Generic 5axis Fanuc post I'll leave these tips for anyone interested:

 

For safe retracts I've found that using limits instead of job setup stock values for retract output calculations works better. Set x and y limits to a value equal to the stock dimensions plus half the toollength amount and use an incremental retract amount in the operations that isn't too big. Set z- limit to 0.0 (or top of stock) and z+ limit to an amount greater than toollength. It's a pain to reset limits for each job but it's the only way I've found of getting good retract clearance for head/head type machines.

 

Spending time looking at the windup limits, axis assignments and signed output variables pays off but what really pays is spending time understanding the machine motion. One of the biggest problems I ran into was solved by simply hardcoding a rotary axis index to zero at program head before any motion began and everything worked after that.

 

The only bug I need to deal with is changing rotary -0.0 output to -360.0 but I might have to deal with it 'cuz I think the solution is buried deep in the .psb file.

 

HTH,

 

steve

[crazy^millman]

Wuold it be Here:

code:

---

#Output formatting

top_map : 0 #Output toolplane toolpaths mapped to top view

#The post must have code added for your machine control

spaces : 1 #No. of spaces to add between fields

pang_output : 0 #Angle output options, primary

sang_output : 0 #Angle output options, secondary

#0 = Normal angle output

#1 = Signed absolute output, 0 - 360

#2 = Implied shortest direction absolute output, 0 - 360

---

This is from a PDF I have:

quote:

---

The primary and secondary axis can be output with the options

of signed absolute output or implied shortest distance absolute

output within the range of 0 to 360 degrees.

The post always works internally with the angles as if normal

angle output was applied (rotary axis windup in a linear fashion)

and manipulates the angle when writing to the NC file based on

these settings.

Rotary Output Options

pang_output : 0 #Angle output options, primary

sang_output : 0 #Angle output options, secondary

#0 = Normal angle output

#1 = Signed absolute output, 0 - 360

#2 = Implied shortest direction absolute output, 0 - 360

---

HTH

[crazy^millman]

JMC my post only put in one unwind. If you do not have a full articalting Head with the full axis movement might be given you the trouble with this toolpath. I also turned on the filter as well as told it to opmtize toolpath and foolw surface in advanced setting turned then 400 line code into about 250 line of code verse the 2400 lines of code doing ti the other way. I would try to limit my head moves to longer moves verse many moves the other way does. I have much better results if the head can make longer fluid movements verse the short jerky movements and have not had less than diserable results doing it that way.

 

HTH

[steve f]

Millman^Crazy,

 

I currently have pang_output and sang_output set to 1 so the post will (correctly) output W-0.0, for example, to perform a ccw rotation to 0 on the C axis. Unfortunately this is the only situation where the machine won't index in the correct direction but always defaults to positive rotation when it reads a zero index position, regardless of the signed address (it even specifies this in the manual). I tried a few things without luck and after thinking about it some more, realized a simple line of logic in the pmx0 postblock would solve the issue. I think this would need a fix right at the source of the code since signed angle output is generated in the psb.

 

thanks for the suggestion though,

 

steve

[crazy^millman]

JMC I just finised up this part today and had the same stiuation as you and here is a file showing how to use Curve 5 axis just like swarf but keep yout tool controlled the way you want. It is Called CRAZYCURVESWARF.ZIP in the MC9 folder on the ftp.

 

HTGAIOWIWDFTP

 

Hope That Gives An Idea Of What I Was Doing For This Part

 

[MIL-TFP-41]

^^^^

 

Good thought there. I will not be able to try it on the machine for a while, but it does follow the path of the swarf toolpath closely (not exactally). The code still still has moves where the C axis reveres itself, tho the moves are gradual and not a sudden reversal that I was getting with Swarf.

 

Still...Swarf should be the way that this part is done. There is an upper and lower rail. Once again I believe that wall gouge checking and swarf do NOT go together. Doing this toolpath with a Curve 5ax mean creating additional geometry, which is not a huge problem....It seems to me that this is a "workaround" for something that does not work the way it should.

[crazy^millman]

Well I create all types of extra gemontry for doing my 5 axis work. My head is very bulky and in certain moves will crash if not truned a certain way. I use line and chains for axis control all the time. I look at it this way what is 5 minutes of gemontry creation verse a dead part or a crashed machine. I say this since we do not have verification software here for 5 axis work and I am using a post I developed from MPGEN5AX_FANUC that does great on alot of things but on others does not. Each indivdiual apporachs thing their own way and if you feel that is your option to do the work I think you piant yourself in a corner. I was trying to show you an alternative for what you were trying to do that might give you a different result. I pass back to you what others have passed to me on here. I again hope it helps and have a good day.