2018 4 axis a simple round part Machine on 3 sides 90 deg rotation

[progaseng]

I've been struggling all day with this I'm lost haas 4 axis vf2

I can get the top tool plane no worries and the second but it won't rotate the part 90 deg

I've tried all I can do in planes managers I know it's a simple solution can you guys pls help

thanks so much .

[#Rekd™]

Can you post a file or at least a photo of the part?

 

 

[Rstewart]

Create planes at respected degrees you want using dynamic planes rotating about center.  When you create a toolpath select that T and C plane when you select your cutting geometry, same WCS.  That should give you an "A" move 

[crazy^millman]

WCS if you main positional location for your programming. It controls your 6 Degrees of Freedom. Six Degrees of Freedom Then we get into the math behind the Post processor we start looking at Euler Angles and Matrix Math.  Euler Angles Those links are those who like me read a lot technical information. 

When you program in Mastercam the WCS allows you great freedom and flexibility to program as many operations that are needed from one model without the need to move the model to different orientations to machine it. On a VMC 4 Axis machine we have normally have the 4th Axis rotating around the X axis and that gives us A Axis output. In Mastercam we set the WCS to the Zero position we want to use when we setup the part in the machine. If you are thinking  the very front of the part then that is where you would place the WCS at if the part is not located correctly in the Mastercam like you need. There are two schools of thought when it comes to programming in Mastercam. The first school of thought is move the model to the position and location you are machining it. The makes copies of that to a new level that will be moved and rotated. the second school of thought is you leave the model where it is and use the WCS to do that work for you. You work with one model, but use levels for your machining geometry and other things needed to machine the part. I got away from the first school of thought around the V9 days, but have used it for different reasons. 

The use of the WCS is what really confuses people from what I have seen on the forum and teaching people Mastercam for almost 15 years. Everyone of us is wired differently and don't get frustrated or aggravated you're not wrapping your brain around the process yet. In Mastercam you need to get a good control over the planes Manager. I use three screens with the main Mastercam in the middle. The planes Manager to my left screen and the operations/solids manager combined to the right splitting the screen with the levels manager. I set all of my work offsets in the planes manger. Since about X7 X8 they introduced Automatic crashing to Mastercam with the useless Automatic Workoffsets if you are doing anything more that a part with four holes it in. I teach everyone set your work offsets in the planes manger. Need to change them then yes there are very easy ways to change them after they are created. The planes manager is your multiaxis control central when doing anything that is 3+1 4 Axis work or 3+2 5 Axis work. in 5 Axis operations you don't have to worry about planes since the 5 Axis operations control everything you need. In Mastercam he WCS is your TOP/TOP/TOP as the part is places on the machine and you're looking at it through the spindle of the machine for a VMC. In Mastercam the WCS is your TOP/FRONT/FRONT if you are looking at the part through the Spindle of the machine. Lets stop right here and break that down. What do you mean TOP/TOP/TOP for a VMC and TOP/FRONT/FRONT for a HMC? Which was is Z when we stand in front of the machine? Z for anyone is always Up and Down and in Mastercam Z for a base WCS is still the same. On the Vertical that seems to make perfect sense, but someone new to a Horizonal machine they think not I must make the WCS the same as the spindle and sorry that is not the way I program and the way Mastercam is setup to handle the machining environment. The FRONT/FRONT are the Construction and Tool Planes in Mastercam. They let the Post Processor know you are machining in a HMC machine and do all the heavy lifting for you when it comes to rotations and multiaxis work. We want to machine at B 90 degrees on a HMC we use the TOP/RIGHT/RIGHT we want B 1180 we use the TOP/BACK/BACK. The WCS has not changed, but the C and T planes have changed. 

The VMC is not different, but we have a machine and control definition made to support our machining environment and again it does all the heavy lifting for us to work with the post to take what we need and convert it to G and M code to run on our machine. We want to machine at A90 then we use TOP/FRONT/FRONT and normally we get A90. The difference here is the Axis of rotation. on the HMC we are rotating around the Z axis so I had to sue the right plane. On the VMC we are rotating around the X axis so I have to use the Front plane. The WCS for that machining operation never changes, but the C and T planes will change for each angle and rotation I am machining if I am using planes to control those rotations. We have many ways in Mastercam to do rotations from 4 or 5 Axis drilling, Transform Rotate Toolpaths to any of the Multiaxis toolpaths. The key is the WCS is your base of operation for all toolpaths related to a setup. Need to machine the other side of the part. Then make a new WCS and name it 2nd Setup or G55 ZERO in your planes manger. Make all of your work from that and keep moving to completion. Once you stop and realizes we always use this process in our daily live from anything like typing on the key board to drinking a soda with our own bodies then we realize we have been programming our whole lives. We just don't think about all the steps needed to make those motions, but break each key type on the keyboard down to CNC code and what your fingers have to do to just type a word and you see how really smart every human is. 

Share a sample part and someone can walk you through the process. The Official Mastercam Website if offering Free Mastercam U classes all you have to do is register on their Web Site to access them. In-House the providers of this Forum have a great resources along with many others out there. There is not need to struggle with so much out there we didn't have when I first got into this line of work. For the most part self taught and don't have a College degree. 

Have a good day and look forward to seeing what can be done to help you progress forward. 

[CristiP]

1 hour ago, crazy^millman said:

WCS if you main positional location for your programming. It controls your 6 Degrees of Freedom. Six Degrees of Freedom Then we get into the math behind the Post processor we start looking at Euler Angles and Matrix Math.  Euler Angles Those links are those who like me read a lot technical information. 

When you program in Mastercam the WCS allows you great freedom and flexibility to program as many operations that are needed from one model without the need to move the model to different orientations to machine it. On a VMC 4 Axis machine we have normally have the 4th Axis rotating around the X axis and that gives us A Axis output. In Mastercam we set the WCS to the Zero position we want to use when we setup the part in the machine. If you are thinking  the very front of the part then that is where you would place the WCS at if the part is not located correctly in the Mastercam like you need. There are two schools of thought when it comes to programming in Mastercam. The first school of thought is move the model to the position and location you are machining it. The makes copies of that to a new level that will be moved and rotated. the second school of thought is you leave the model where it is and use the WCS to do that work for you. You work with one model, but use levels for your machining geometry and other things needed to machine the part. I got away from the first school of thought around the V9 days, but have used it for different reasons. 

The use of the WCS is what really confuses people from what I have seen on the forum and teaching people Mastercam for almost 15 years. Everyone of us is wired differently and don't get frustrated or aggravated you're not wrapping your brain around the process yet. In Mastercam you need to get a good control over the planes Manager. I use three screens with the main Mastercam in the middle. The planes Manager to my left screen and the operations/solids manager combined to the right splitting the screen with the levels manager. I set all of my work offsets in the planes manger. Since about X7 X8 they introduced Automatic crashing to Mastercam with the useless Automatic Workoffsets if you are doing anything more that a part with four holes it in. I teach everyone set your work offsets in the planes manger. Need to change them then yes there are very easy ways to change them after they are created. The planes manager is your multiaxis control central when doing anything that is 3+1 4 Axis work or 3+2 5 Axis work. in 5 Axis operations you don't have to worry about planes since the 5 Axis operations control everything you need. In Mastercam he WCS is your TOP/TOP/TOP as the part is places on the machine and you're looking at it through the spindle of the machine for a VMC. In Mastercam the WCS is your TOP/FRONT/FRONT if you are looking at the part through the Spindle of the machine. Lets stop right here and break that down. What do you mean TOP/TOP/TOP for a VMC and TOP/FRONT/FRONT for a HMC? Which was is Z when we stand in front of the machine? Z for anyone is always Up and Down and in Mastercam Z for a base WCS is still the same. On the Vertical that seems to make perfect sense, but someone new to a Horizonal machine they think not I must make the WCS the same as the spindle and sorry that is not the way I program and the way Mastercam is setup to handle the machining environment. The FRONT/FRONT are the Construction and Tool Planes in Mastercam. They let the Post Processor know you are machining in a HMC machine and do all the heavy lifting for you when it comes to rotations and multiaxis work. We want to machine at B 90 degrees on a HMC we use the TOP/RIGHT/RIGHT we want B 1180 we use the TOP/BACK/BACK. The WCS has not changed, but the C and T planes have changed. 

The VMC is not different, but we have a machine and control definition made to support our machining environment and again it does all the heavy lifting for us to work with the post to take what we need and convert it to G and M code to run on our machine. We want to machine at A90 then we use TOP/FRONT/FRONT and normally we get A90. The difference here is the Axis of rotation. on the HMC we are rotating around the Z axis so I had to sue the right plane. On the VMC we are rotating around the X axis so I have to use the Front plane. The WCS for that machining operation never changes, but the C and T planes will change for each angle and rotation I am machining if I am using planes to control those rotations. We have many ways in Mastercam to do rotations from 4 or 5 Axis drilling, Transform Rotate Toolpaths to any of the Multiaxis toolpaths. The key is the WCS is your base of operation for all toolpaths related to a setup. Need to machine the other side of the part. Then make a new WCS and name it 2nd Setup or G55 ZERO in your planes manger. Make all of your work from that and keep moving to completion. Once you stop and realizes we always use this process in our daily live from anything like typing on the key board to drinking a soda with our own bodies then we realize we have been programming our whole lives. We just don't think about all the steps needed to make those motions, but break each key type on the keyboard down to CNC code and what your fingers have to do to just type a word and you see how really smart every human is. 

Share a sample part and someone can walk you through the process. The Official Mastercam Website if offering Free Mastercam U classes all you have to do is register on their Web Site to access them. In-House the providers of this Forum have a great resources along with many others out there. There is not need to struggle with so much out there we didn't have when I first got into this line of work. For the most part self taught and don't have a College degree. 

Have a good day and look forward to seeing what can be done to help you progress forward. 

Nice post man!!!! Pleasure to read it.

[AMCNitro]

From experience... Is your post 4th axis enabled?  You can have all the planes perfect, but if your post is only configured for 3 axis it will never post the rotations

[progaseng]

Yes it’s 4th axis enabled as I was able to do engraving etc . It’s a simple part could be any part where u rotate 90 so front back bottom top etc I have mr datum sat centerline of part left side with axis on right side as typical thx 

[crazy^millman]

56 minutes ago, progaseng said:

Yes it’s 4th axis enabled as I was able to do engraving etc . It’s a simple part could be any part where u rotate 90 so front back bottom top etc I have mr datum sat centerline of part left side with axis on right side as typical thx 

Take a screen shot of the operations Planes page and post it up. 

[progaseng]

I figured it out I had to turn rotary to off and then put a zero in for work offset works like a charm now thx all for your help . Ps why do I have to put a zero in for each tool plane offset ? Default is -1 

[Leon82]

-1 is automatic and it makes a new offset when you make a plane. 

 

Setting it to 0 keeps it g54

[progaseng]

Perhaps someone can give me a sample of how each works as I’m unsure ? Thx