Quintax 5-axis router

[wildcat99]

Our first machine, a Quintax 5-axis with twin 5x5 tables and a xxxxor 8055 controller has arrived! The Quintax rep will be here this week for setup and training.

 

Is there anyone out there using a similar Quintax/Mastercam combo that would be willing to share their experiences? Any advice on what to expect, what to look out for, what questions to ask, etc?

 

This is my first introduction to CAM and CNC. To start with we will be trimming large, molded plastic parts held with vacuum fixtures. I have 4 parts programmed and the pressure is on to make this machine productive ASAP. I guess I'm a little nervous since the true "verify" occurs when the first part is cut. Any advice from experience would be appreciated. Thank you.

 

[ 02-11-2002, 12:46 AM: Message edited by: wildcat99 ]

[Travis_Buchanan]

Wow. First machine is a 5 axis. Do you have any previous cnc machining experience? Seems like you all just skipped the whole bottle feeding and baby foods stage in the game. Our first machine was a 1964 2.5 axis tape feed router. No g code what so ever. Only 4 M codes, spindle up, spindle down, depth turret advance, & program end.

Programming was all incremental and the sum of all x & y values had to be zero, so your program didn't float off the part. Just a bit of trivia.

--

Buzz

[wildcat99]

Buzz:

 

No we don't have any previous CNC machining experience. The closest thing we have to CNC is our automatic bandsaw and a pen plotter.

[Zero]

Sounds like a 'crash course' to me(just the way I like 'em).We're supposed to be getting our controller on the network today.No more being limited to 1.38m files anymore!!!!!Now I just gotta get the boss to get a machine with a tool changer and a 4th(maybe 5th) axis.

 

Good luck dude.

[Mark H]

The next thing that you will need (if you dont already have it) is a 5 axis post to go from Mastercam to the machine.

[mold100]

wow,Ive been thrown into the fire before,but your into a blazing inferno.No 5 axis expierience here,just saying goo-luck.Sounds like an intersesting challange.

[mold100]

oops, I mean good-luck.

[cadcam]

Wildcat99,

so you know, and I think you know it but we are all here to do our best and help you along.

 

I all so sugest getting with your local dealer to.

 

Also what Mold100 said.

[ERIC14779]

wildcat,

 

Welcome to the Quintax club it is nice to see that others value rigid router construction. I haven't spoke with Denny at quintax lately but they do have a post that works sort of OK but they were working with CNC software to get it better. We have had our dual table 12 Hp 40 taper 5x5 machine for almost a year and have done many things. 5 axis programing is hard sometimes but like others have said they can help out on this forum...

 

Contact me via my e-mail if you need to discuss anything in regards to your new machine.

 

AND REMEMBER keep one hand on the feed override. And both EYES on the machine when proving out a program.... Start slow then cautiously speed up.

 

Good luck

[wildcat99]

Thanks for the replies. Some of you guys scare me!

We do have a 5axis post from our dealer that is ready, but we need to provide the pivot length of the spindle as it rotates in the B-axis. We are going to try and measure that today.

With our first complex parts, we are probably going to do a dry run with no tool to prove out the program and also test the post.

How does everyone else prove out their programs?

[ERIC14779]

wildcat

 

the method I use to figure pivot length is:

 

set a indicator (1" or better travel) on one of the tables and set B to + or - 90 degrees with a tool in a collet chuck bring the Z down( on the tool shank) to the indicator (note that the Z will only come down to about 12" above the table at +or- 90) set the indicator to "0" then at the control preset Z to + half of the tool dia. (ie. if you have a 1/4" shank tool set Z to +.125) then crank Z up so the tool will clear when you rotate B back to 0. Then rotate B back to 0. and move X and Z till you can bring the tool tip down onto the indicator tip and bring Z down till the indicator shows the same 0 as when you had B at 90.

 

look at the coordinate display at control the number shown is your total pivot length.

 

then set your Z zero as you would in 3 axis mode along with X and Y.

 

when you post your operation with Mastercam enter this total pivot when asked and you are ready to prove out the program.

 

[ 02-12-2002, 03:52 PM: Message edited by: ERIC14779 ]

[Claus@Cimco]

I don't understand why you have to give the toollenght to the postprocessor, normally the xxxxor 8055 is using TCP(Tool Center Point) to compensate for this. that means, if you have the right lenght of the tool in the tool register on the control ( lenght from spindelnose to tooltip). and the control is setup right (distance from pivotpoint to spindle nose). Then the ncprogram only needs the coordinates for the tooltip and the B and C angles. Then the control will compensate for the toollengt + the distance to the spindelnose from pivotpoint.

The good thing about this is, now you can change the tool without postprocessing a new program for every new tool lenght.

TCP is made active by G48S1 and inactive by G48S0

But all this is descript clearly in the xxxxor 8055 manual/CD (chapter 17.3 in the 8055musr.pdf).

 

Claus@cimco

[wildcat99]

You guys are good. Bear with me if I ramble or don't get the terminology quite right.

 

Eric: Todd with Quintax did exactly what you explained to get a total pivot length. Do you have to re-post the program with a new pivot length when you replace a tool? Do you have to manually measure any tool lengths?

 

Claus: Do you have to manually measure the length of the tool in the tool register(spindle nose to tooltip)? Apparently we don't have the TCP G48 option on our control. We are going to find out if we were supposed to get this. It sounds like we should have for what we are doing. We also don't have our xxxxor manuals yet, but we have a machine...go figure.

 

Our dealer originally set up the post to where he would hard code in the pivot length (distance from the pivot point to the spindle nose). Then we would enter in a tool length (length from the spindle nose to the tip of the tool) when posting in Mastercam. To get this, he suggested using a height gage and measure from the flat part of the toolholder to the tooltip with the holder in a gage block. The toolholders don't fit flat against the spindle nose, there is a gap, so I don't see how this would help in total pivot length anyway??

 

Also, we have a toolsetter on the machine (a sensor that the tool touches off on) if that makes any difference. I understand we will run this routine each time we add a new tool to the tool changer. Thanks for the input.

[Travis_Buchanan]

Wildcat,

 

How about asking the machine dealer for the distance. Im sure they can tell you, and if they don't know they should be able to find out. I asked a machine dealer recently and he did not know, but the next day I had a fax from Japan with all the infro I needed. This will get you a good accurate number and will save you some time.

Good luck with your machine, these guys/gals here on this forum are very helpful to each other, and I was just yanking your chain about skipping the bottle feeding and baby food stage of the game. I think if you get started off in the right direction with a little help from some experienced 5-axis people you will do just fine.

--

Buzz

[ERIC14779]

wildcat

 

tell todd I said Hi.

 

If you do not need real tight tolerance you can measure the overall length of the tool & holder from the retaining stud to the tool tip and when you put in a new tool make it the same. or if all of your collets are from the same mfg. you can measure tool stick out from the face of the collet.

 

I do not know with the presetter this all may be mute as it may be able to calculate the pivot length for you... I dun-know...

[Sem001]

If you are using a tool changer why not set up a standard that you can use to guage where the part is at a known length then put tool in touch off using the same height offset and offset the difference may save time against guaging each tool individually

[wildcat99]

OK. Here is where we're at.

Our toolsetter will give us the total pivot length for each tool and place it in the tool register on the control. We take this value and enter it into Mastercam when posting. If we break/change a tool we toolset again and repost.

 

If and when we get the xxxxor TCP option, the control will actually be able to use the values in the tool register. No need to enter pivot length values in Mastercam or repost. The control will automatically adjust for new tool lengths.

 

Thanks for all your comments, it helps to see how someone else is doing things.

[ERIC14779]

wildcat

 

won't you still want to have the tool sticking out about the same distance on a future run so you do not have clearance problems with collet nut ect. ???

 

I still would record the approx. stickout for each tool for a job and record it in the progarm as a REM statement.

 

I do not like to do any tool comp in the control at all. It is to easy to have the wrong numbers in there for the tool that you are using.

 

Unless the tool presetter verifies the tool length before the machine starts to use it???

 

Be very carefull.. If your work is like mine (Many different parts) smaller runs (1 to 5 days) then another job... I would suggest putting the proper pivot length with a known tool stickout in the post and let the post calc. where the tool tip is. then prove the program out and run the parts.

 

A extra 15 min. calculating pivot length by manual methods (untill you get a set procedure) my save a busted machine or fixture.

 

JMTC

[ERIC14779]

Wildcat.

 

How did your install go??

 

Have you cut any parts yet??

 

Are you feeling anymore confident(sp)

 

How is your post working ???

[wildcat99]

Eric

The install went OK.

 

We did a teach-in program to trim off flash and mill 10 holes on a simple part. Since Todd left we have cleaned this program up a bit and it works great.

 

Confidence....still shaky.

 

5-axis post...not working, major modifications needed.

 

I am learning more than I ever desired about g-code right now.

[ERIC14779]

yep

 

That is how it went for me too....

 

Especially the part about learning G code never had to before Mastercam did all the work.

 

That teach pendent is something to learn how to use for arc moves. FYI if you are programing something only on the V table you must have both tables active (M60) as the teach in will not output V axis moves only X,Y,Z,B,C... then put in a G28 YV to swap Program Y moves to the V axis.

 

don't give up just go slow and carefull.

[woodbutcher]

Hi Wildcat,

 

Just wondering how things are going with the new Quintax router? I am very close to signing on the dotted line with them for a 5 axis machine and would appreciate all input from this forum. I am also real concerned about all these post problems I read about. Did anyone get there post from Quintax and still have problems? Or are these problems coming up when you go through your local dealer and have them supply a post?

[ERIC14779]

woodbutcher

 

We got our post from Quintax but they got it from one of their other customers who modified the mastercam std. 5 axis post.

 

They are working with a Richard Taft at CNC Software to get a bulletproof post for their machine but it is going very slow for them.

 

Also I think that most of thier customers are not asking for a MC Post and are hand programing or getting by with what they got.

 

I have been asking about the post and dont get far. Mabe if more people who have or are buying a Quintax would make a bigger (stink) about a MC post it would become a bigger priority???

 

I even volunteered to test the post and give feed back directly to CNC Software to get it done for us all.

[Claus@Cimco]

Hi

A easy way to see if TCP is enable or not, is to check the parameter P93, if 0 TCP is disable. 2 is for a dual swivel spindle and 3 is for a angled spindle.

On a dual swivel spindle the parameter P97 holds the distance from the pivot to the spindlenose. This value should not be 0.

I have made a 5axis post processors for this control ones in Akron, Ohio, a dual swivel type. The Quintax is new to me, but I think it must be a simple task for a 5axis Post Processor programmer.

 

Best Regards

Claus@Cimco