5 axis trunion c axis solution

[dolphin1]

trying to find out about the c axis break program and rotate for when you exceed the y+ axis limit.this is for a Mazak Variaxis 500 and only has 6.1 inches of y+ travel.right now i have to program the features in y- and hand write in the c axis rotation value.ive tried this in t/c planes but it doesnt work.

 

any one know a work around for this other than buying another post.also this is when the a axis is at zero degs.the post i have now will do it if there is a a axis value other than zero degs.

[crazy^millman]

If you bought a post and it does not do what you want then I would be raising some major cane!!!!!!!!! I wonder how you are approaching your plane set-up for your limits. If you only have a 6-1/2" Y axis travel and are programming 12" cut no post is going to fix that for you that I know of. Our Integrex has a very little travel below Zero in the X direction and if I program the machine to cut below that it is my fault and not the posts. I need to keep my limits in mind when programming and approach work for this machine with that in mind. I have 6 jobs I am doing right now. One is a rectangle block and I am doing half the block with the spindle indexed at A0 then doing the rest of the block with the spindle at A180. I needed to brake up my chains keeping my limited X axis travel in account once I did that all is good.

 

With that said I am not saying it is not a post problem, but unless you got some sample stuff to post up and example file for someone to judge for themselves then I am going to be on the fence as to the problem, because IN-HOUSE is the only people I trust to buy a post from for these types of machine and you are slamming someone who you bought a post from and seriously doubt they are unwilling to help you.

[dolphin1]

well the post was writen by cnc software.the variaxis has more travel in the minus direction than the positive.y+ 6.1 and y-13.98 basicly.the problem i was told is there is a infinite possibly solution with the a axis at zero degs and this is the prob.if there is a angle on a axis then the solution is usually a single one which makes it more simple.

 

a simple example is doing a 15 inch bolt pattern where some of the holes run out of travel in y+.then you have to pick the holes that would normally be in the y+ area and make them the opposite in the y- area and post the prog and hand write in the c axis rotation value to run the part.

 

ive got a quote from In House but the company doesnt want to spend the money.just trying to see if there is a work around im missing.

[crazy^millman]

In that case I would do part of my bolt circle using one C-plane and then another C-plane to do the rest. I have the same problem on our Integrex and get around it, by this very method. If you would like to send me a file I would be glad to take a look and see if I can give you a solution that would work for you. I would still be on the phone to someone at CNC everyday until the problem got resolved. If push came to shove, I would make a misc integer that would output my index so I could have something outputted the same way everytime.

 

HTH

[sherwood]

Hi Mike.

We use the Variaxis 500 as well.

I can only suggest you would pick the hole positions that you know will not overtravel - in the y- positions - in one toolpath then pick the hole positions that you know will overtravel in the next toolpath but in the second set of holes you can use the miscellaneous values button - uncheck the box for auto post settings and enter the default angle for rotating axis to 180.

Post both toolpaths and the second set of holes will have a c rotation.

Regards.

Ian.

[dolphin1]

Ron i will send a file on monday after i send it home as we lost internet at work.im not sure i follow on the misc interger method but will play with it more.not sure what good calling cnc would do but i will contact my reseller again.

 

Sherwood still dont understand using the misc int in this case.will look on monday and see if i can figure this out.

[dolphin1]

quote:

---

In that case I would do part of my bolt circle using one C-plane and then another C-plane to do the rest.

---

well you have mail.i did try to do what you said earlier but it posts out zero deg's on the c axis.

 

as for creating a misc interger im not real good on post stuff but i will try to see if i can figure it out.after reading this again i think i understand better.

 

quote:

---

uncheck the box for auto post settings and enter the default angle for rotating axis to 180.

---

after checking today i have the box unchecked anyway.where do i add the default angle.

[crazy^millman]

Mike never got a file.

[dolphin1]

ok well i dont know what happened but i sent it again.hope you get it and so you know its a zip2go.

[crazy^millman]

I got both files and will look at it for you tomorrow.

[crazy^millman]

Ok as I thought. It is your approach to the whole concept. C-planes control your indexing. You had one C-plane at 180. I made 2 more indexing C-planes. One at 90 and another at 270. I then broke up your 1st operation into 4 operations and the 1st operation has 2 holes at top, 2 holes at 90, 1 holes at 180, and the last 2 holes at 270. Try this post it and see if your machine alarms out again.

 

I assume you know how to rotate C-planes so I did not cover that. If you need help understanding it better let me know.

 

HTH

[dolphin1]

when i set up the part i tried to get it to rotate the one hole that was out of range.all it would do was post it out at the same place and no rotate.

 

i will look at the stuff you sent tomorrow as it didnt come through before i left work.

[crazy^millman]

Sorry I did not send anything. I can I just did not have the time. I will try to have you something before I leave today.

[dolphin1]

ill be watching for it,thanks.

[silky_johnson]

dolphin1,

 

I don't know if this would help but I used to run a Mikron UCP1150 that had the same issue, all the Y travel in one direction. It had a specific M code that would activate a retract and would rotate the C axis 180 degrees so that the Y- was now Y+.

 

Of course, different machine and different control, but you might want to contact Mazak to see if they have a solution on the control. My bet is if the machine only has that much travel in a particular direction, then there must be a control solution as oppose to a CAM or post solution.

[Jim at Gentex]

I have a similar situation with my Deckel Maho with the external type of rotary table. The rotary table is mounted to the right side (X+) of the main table, so this gives me very little X+ travel past the center of the rotary table.

 

When that happens, I do exactly as Ron suggested.

I use different Cplanes and / or different fixture offsets to reach anything beyond the X+ travel limit. (i.e., rotate the table 180, then X+ becomes X- )

 

Once you get the hang of it, you will be OK.

[dolphin1]

well i got to say you guys had me to a point where i thought i didnt know how to do this.tried everything i know to get this to work and i finally asked my reseller about this.

 

well it turns out that my post wont do C-axis rotation from c-planes unless there is a A-axis angle involved.my reseller tried to do what im trying to do and he said he tried everything he knew with the post and could not get it to work.

i guess the solution wasnt avail when we bought our post.

 

the post he got me a quote on from In house will do it just fine but i never got time to play with it and its allready timed out.oh well i guess ill never get to do this other than hand writing the solution as my company wont spend anymore money since i have a perfectly good post they allready paid for.

 

so here is to all the people that tried to help,Thankyou very much and i hope some day i will get to use a real post.

 

Thanks.

[silky_johnson]

Still think there should be a machine/control solution...have you called Mazak?

[crazy^millman]

Mike contact Jim Evans at CNC and see what he can do. Contact Pete, John, and whoever else works there. Get on the phone and become the biggest pain in the neck. Then get a lawyer and let him become a big pain in the neck. They need to give you your money back so you can get the IN-HOUSE post. I was in a similar problem as yourself though not with CNC and got it resolved to everyone's liking. There is no reason why you should not be able to do what you need using Mastercam. You paid for it and it does not work and that needs to be addressed.

[dolphin1]

quote:

---

Still think there should be a machine/control solution...have you called Mazak?

---

ive got one of the techs working on it for a while but nothing yet.

 

as for contacting cnc software im working with my reseller.