3+2 question

[DavidB]

I was shown to rotate my job around the rotation axis of the machine to a position that is required to machine a feature,save it to a level named what ever the rotoation is.

I then use misc interga to put in A angle B angle in the program.

My question is if i leave modal and create a toolpath using a toolplane can i get a post to output the A&B rotation angles.

Our is this the preferd method?

The post would have to know where the rotation point was.

The machine in question has a rotary wich rotates around Z 360° which is on a rotary which rotates around Y axis +90 to -90.

The rotation point is 90mm below X0 Y0 Z0.which I set to top and centre of rotary table.

Hope I made myself clear.

Thanks in advance

[crazy^millman]

Well David what I would do is leave the part alone and just create a C-plane from that working surface then your post should output the correct index angle. The trick is to make sure your x axis is facing the right direction. It is you lok at OCTOGON TRANSFORM in the MC9 folder you will see that I did this simple part in 2 ways one way was to use Cplnaes for the 8 sides and when you post it the index moves are done autotmacilly. The others was to take the first operation and then d oa transfrom rotate around the center axis or the origin to create the other toolpaths in the 2nd group. This is my test program for post that I work on. If they do all of that right and do the clearence correct then I feel pretty good about the post for the shop.

 

Now option 2 that is to use the MISC to do manunal indexing. If you look in the simulate index moves in Mpmaster that I responed to this week I have a very good example how to do this very thing. Link to thread: Manunal Index in Post. That example used lock codes for the 4th axis from a Fadal but can take them out or change them for the machine you have there.

 

HTH

[DavidB]

Millman thx for your responce i cant acsess the FTP site at work could you email me the example please [email protected]

I only now the way mentioned because thats what I was taught,but since i bought the Mastercam hand book Volume 3 (5 axis)I have been thinking about it a lot more.

 

Your op 1 sounds like what im thinking,how does the post now where the rotation point is?

 

Thx again

[crazy^millman]

David I will send it to you tommorrow when I get to work.

 

When you have a part where the center line of the part is at the origin and the end of the part goes along the same point or any center point of rotation depending on the part this is where every thing begins for programming on a 4th axis or a horitzonal machine. The octogon is a good exmaple becuase it has 8 sides. With these 8 sides we have 360 degrees being a full circle with 8 divisions of that being the places where our faces end up when the indexer moves to put the face normal to the VMC or HMC cutting plane which depending on the side is a 45 degree increment from 0 degrees. Every time you pick a c-plane the program is looking at a 3 point place to understand where that is reative to the WCS which I always use one and nothing else for 4th and 5th axis toolpaths. The idea of Quadratic Equations and the cartesian coordiante systems comes into play. Where 3 point are defined and make a plane that is where the Mastercam knows that place in space and make the determation of the angle in realtion to the place it started. In my simple thinking if you go throwing multi WCS places into Mastercam in essesnce you are make the place you started in space lost so that everything else can be realtive if you where to use c-plnase for those WCS places. You would need to use only WCS for every where you wanted to go or you would need to use ony one WCS and the use the C-plane as your plane control for the places realtive to the start point. The thing here is that with a 4th axis machie all of the those planes need to share the same parrelle plane that is X axis but but be rotated around that same place for the post to understand what you are wanting to do. If you are thinking about how Mastercma looks at rotation and how you would look at rotation it is the same the problem is that we assume that is selecting a certain face that we rolved around the same place when we did not we did not keep the X axis going in the same direction and that is X postive going to the right as with and standard quadrtic equations and using cartisen coordiantes. This is the dreaded only one axis of rotation is allowed so many of us get when doing 4th axis work. I have found it best when doing any machining to be the endmill doing the work. I imangine myself doing the cutting and the work and then look at the screen and see if I am being told the same thing every time when looking down from the place I am cutting if that be with a angle of 0 dgrees or an angle of 97.2375 what direction is my X postive going and is it going right which is postive or left which is the wrong way or is it going up or down or off in some crazy direction this how you see where you have made your mistake. I have moved parts to the right place just like you and I have moved my C-plane to the same place and that is all you are really doing by moving the c-plane to the right place you are mving the place where Mastercam is being told to do it work where you need it to much like moving the part you are just moving the place where Mastercam sees that part and how to do the operation for that. This is where the post takes over it takes the data from Mastercma and see that plane in which you have made the c-plane and throuh calucations in the post understand what you have told it and says ok since I have been told this WCS or C-plane is rotated arond the center of X axis I need to move something there and the posts knows it can not move the head so I have to move the machine and when you have a post that does 4th axis it moves the A axis to that place and now it understand that you have that posted operation of code in the correct place and makes all of it normal caluaction as if nothing was different than programming from the top plane and when you really think about it you are all the time working from the top plane when making it on the vertical machine but the trick is to get Mastercam to see it the way you see it on the machine and once you have that down then you see the whole idea behind the use of more than one WCS or the idea I use of one WCS and different c-planes. Sorry for the length and sorry for the bad spelling and typing but hope you got what my humble idea is of what is going on here is.

 

This is just my opinion and I only offer it as that nothing more nothing less. He is affarid to make mistakes in life never learns and he who makes the mistakes and learns keep on learning.

 

Let us all have a good week.

[cadcam]

Daved what type of machine is this?

this shounds like you added a dual rotatry table to the virtical.

 

So you should be able to at least do 5 axis postioning.

 

So following some of Millman I would create named views in the WCS and the set the Tplan and the c-plan when wanting to use that named view.

 

do not set the WCS to it, just set as stated. If your post is set correct you will be able to get A&B postioning you need.

[DavidB]

The can do 5axis work its a vertical.

 

I was shown the method of moving geometry by rotating around the pivot point of the machine then programming it in top T/plane and C/plane then adding the angles that i moved geometry into the Misc Interga boxes.

 

I have been thinking to leave geometry alone and use C/Planes but I can only asume the post must now where the pivot point of rotation is relative to my origan.We always set X,Y,Z zero to centre of rotary table and top.I know the rotation point for A will be X,Y,Z zero and B axis rotation is 90mm below origan.A rotates around Z axis and B around Y axis.

 

 

THx

[DavidB]

CadCam i took some digital pics of the machines rotary set up.How do I get them onto the forum?

 

[Glenn Stephens. from CCCS]

You'll need a 5-axis post to get the angles from the c-plane/t-plane (even if it's just indexing).

[DavidB]

Glenn,

Should i continue the way I am by moving Geometry or get a 5-axis post?

 

You have confirmed what I was thinking.

[cadcam]

David you will need a post as Glenn has stated.

As for you pictures you need a place to host them or put them on the ftp we will all view the setup from there.

[crazy^millman]

We have a winner being a 5 axis capablity with that you need the prize of a 5 axis post. Good luck in your search.

 

Contact the guys and CNC automation here is Pierre's email: [email protected] he is a good guy and they do good work.

 

HTH

[DavidB]

I put the pics on the ftp site under all_pictures.picture 019 and 020 dated 6/7/04

 

Should i keep going the way I am or get a 5-axis post???????

 

Im getting the jobs done but what do you think is the better way to do 3+2 programming???

 

 

and Thanks

[cadcam]

axis post makes life much easer and less mistakes.

[cadcam]

I would say after looking at the pictures a post would make that sweet.

I like using the dove tail setup in the multy axis confg.

[gcode]

DavidB,

A dedicated post is definitly the way to go with that machine. Once you get it proved out and learn to use it, you'll wonder how you ever did it any other way.

 

Glen wrote one for my company for this machine Mitsui Seili HU50A-5x

 

Its a full 5 axis post, rotating B on a titling A

It took a little doing, but its nearly bullet proof now. If you look at the picture, the machine origin and the MC origin is the intersection of the rotary table C/L and the tilting axis C/L.

We program in Mastercam, verifiy with Predator VCNC and we're doing some pretty trick stuff with it now.

 

 

If you are just doing 3 plus 2 work you can probably make a good start on a 5X post by modifying the Gen5X post on the install disc.

Tha is what Glen started with for my Mitsui post,

but he had to do some stuff inside the binary file to get the rotary table to work right.

[DavidB]

I know if i ask for a post i'll get YELLED at but is there a post I could have a look at that would give me a good start??

 

I bought the Volume 5 Mastercam Handbook and it got me thinking different than what i was shown (taught).

 

Thanks for the reply's

[crazy^millman]

MPGEN5AX that is on the CD would be a start but that si not an easy post to get tweaked and requies a good knowlegde of posts in my humble opinion to get right. I if had the right post would program everything like I said before one WCs and then different c-plnaes for the places you want ot do thew work and then you would get everything posted perfect. There is this in the post about how ot set it up:

code:

---

#Machine rotary routine settings 

mtype : 2 #Machine type (Define base and rotation plane below)

#0 = Table/Table

#1 = Tilt Head/Table

#2 = Head/Head

#3 = Nutator Table/Table

#4 = Nutator Tilt Head/Table

#5 = Nutator Head/Head

---

I am thinking you would use the 0 which is Table/Table then there are these for setting the distances from one axis to the other in this section:

code:

---

#Axis shift  

#Part programmed where machine zero location is WCS origin-

#Applied to spindle direction, independent of RA

#Table/Table -

#Offset of tables to secondary axis relative to machine base.

#Tilt Head/Table - Head/Head -

#Part programmed at machine zero location-

#Offset in head based on secondary axis relative to machine base.

#Normally use the tool length for the offset in the tool direction

saxisx : 0 #The axis offset direction?

saxisy : 0 #The axis offset direction?

saxisz : 0 #The axis offset direction?

 

r_intersect : 1 #Rotary axis intersect on their center of ratations

#Determines if the zero point shifts relative to zero

#or rotation with axis offset.

---

Don S was working on a Trunion post for his HAAS machine and I think there where the key oy getting it right. These are just my opinion and use this information that it hopefully helps not hinders.

[Glenn Stephens. from CCCS]

There is a powerpoint presentation available that tells you how the gen5x post works.

 

I've put in on the FTP in Text_&_post_files_&_misc. It's called 5 Axis Generic Post.pps

[gcode]

There used to be a Word file that gave some of that info, but I lost my copy of it.

[DavidB]

Thx guys I will put the post on my PC from the Mastercam CD today.

We have two of the machines I took photos of with the pivot point 90mm below rotary table and another similar a Makino GF6 which has a pivot point 111mm below the rotary and off set in the X axis of machine by 75mm.

 

Glenn,thx i will have a look at the presentation.

 

thanks for all replys

[DavidB]

Got the 5axis training guide of the FTP site Cheers.

 

Going threw the post (GENMP5AXIS fanuc) I think it is set for my Machine,correct me if im wrong.

TableTable with primary axis rotating around Z and secondary axis around Y

 

My top rotary which rotates around Z.Will be the primary axis.

The secondary axis rotates around Y.

 

There are some isues I can forsee.

 

1,The rotary that rotates around the Z axis (360°)needs an A put out not a C for rotation angle.

 

2,The B angle which rotates around Y is limited in its amount of rotation.Im sure I can set this Im just not that far into it YET.

 

This is just the start im sure but im looking forward to finally learning about posts.

 

Thanks to all

[gcode]

Change your axis labels here

 

# --------------------------------------------------------------------------

# 5 Axis Rotary Settings

# --------------------------------------------------------------------------

#Assign axis address

str_pri_axis "C"

str_sec_axis "A"

str_dum_axis "B"

[DavidB]

Thx Gcode

 

This is tacken straight from the standard post.

Do you agree it it set for Primary to rotate around Z axis and Secondary to rotate around Y axis.????

 

 

#Primary axis angle description (in machine base terms)

#With nutating (mtype 3-5) the nutating axis must be the XY plane

rotaxis1 = vecy #Zero

rotdir1 = vecx #Direction

 

#Secondary axis angle description (in machine base terms)

#With nutating (mtype 3-5) the nutating axis and this plane normal

#are aligned to calculate the secondary angle

rotaxis2 = vecz #Zero

rotdir2 = vecx #Direction

 

 

In the training notes it says:

The primary rotation is defined by selecting the gnomon vector that defines zero and assigning it to 'rotaxis1'

 

What does gnomon mean?????

 

thx for replys David

[jplecan]

Hi David,

I've used the mpgen5x pst for a horizontal machine with a tilting rotary for 5 axis positioning and also rotary feed on fixed tilt angle toolpaths. The changes I made in the post were

 

mtype:0

 

rotaxis1= -vecy #zero

rotdir1= vecx #direction

 

rotaxis2= -vecy #zero

rotdir2= vecz #direction

 

Experiment with those combinations and I think you'll find what you're looking for.

 

As long as you're just positioning and not doing

5 axis toolpaths, you should be o.k. without the axis shifts (I'm still trying to figure that out,

will take a look at the .pps file soon)

 

Jim

[jplecan]

Jay,

I can't seem to access the 5axisgenericpost.pps

file from the Text&Post folder on the FTP. (page not found) I can get to stuff in the MC9 folder, though. If anyone could email to me, my addy is [email protected]

 

Thanks,

Jim