Right Angle Head Post and Machine Definition Help

[Rotary Ninja]

We have a right angle head coming. We have a part that requires a 3D contour or a surfacing toolpath be done from the ID of a 30" ring. I was told by a colleague that I could modify our 5 axis machine definition to make it work for using a right angle head. We went through our machine definition over the phone and he said I have the right component setup in our Haas 5-axis definition. He said in the toolpath Misc Values page to set the Right-Angle head angle to -90 which works for his setup which is the same as ours. But that's all I got from him. Is this the proper way to do this? How do you go about programming this way?

 

I am being told by our reseller we need to buy a new post and they need to setup the component for us. I am somewhat familiar with editing posts making minor changes. I can't see this needing a completely new post to get this done.

 

If someone could point me in the right direction to make this work I would really appreciate it. I would like to get this taken care of myself if possible.

 

Thanks.

[Colin Gilchrist]

Try looking in the Post Development section of the forum. I just covered some questions about this. The Generic Fanuc 5X Mill Post has some options for RAH work that are activated using the MR values only. Nothing is read from the MD, and the Aggregate Head components/stations are not needed (don't work) with the Gen Fan 5X Post.

 

Basically, the Gen Fan 5X Mill Post has options in the MR Values (MR2 and MR10) that let you flip the cutter 90 degrees (either + or -) about the Secondary Axis.

 

This really only works if you have a Gantry machine (head/head) or a Head/Table, and the "Head" has the "Secondary" rotary axis.

 

You will not have any kind of simulation/visualization of the RAH attachment. You will only get the Tool/Holder shown, performing the RAH cutting moves. This is still fairly "limited" in the scope of what you can do with a RAH in a 5X machine. The Post will handle the offset from the Gauge Line of the spindle, to the tool tip. That is what the MR values are for. For the NC code, the Post will typically take the OAL length of the Tool Definition as the X or Y offset from Gauge line (depends on how your Secondary rotary axis is setup) and will use the MR10 value for the "offset" in the Z axis. (spindle axis).

 

Again, you are fairly limited when setting up and using a RAH attachment. There is much more support built into the software if you are only doing 4X work with a RAH, and you modify a Router Post for use in Mill. Then you can use the Aggregate component in the Machine Definition, and setup the "stations".

 

There are a couple 3rd Party Post Developers (In-House and Postability) that are offering services to "hook up" the output of the 5X Post to run Machine Simulation in Mastercam. Technically, it is possible to customize and manipulate the CL file output that "drives" the simulation to include a RAH, and even make it simulate properly. From what I've seen, this typically doubles the cost of the post. I would expect to spend several thousand dollars for just the Simulation portion of doing RAH work on a 5X post. (If you want to be able to simulate it inside Mastercam, and don't have Vericut! or NCSimul)

[Rotary Ninja]

Sorry, my post was a bit misleading. We are actually running this part on a VF6 with a rotary facing vertical. I was told I could modify the 5x def to make this work.

[Colin Gilchrist]

Ok, so you are running a 4 Axis machine, and want to use a RAH on this machine? Is the RAH programmable? If yes, what does the code look like to rotate the tool?

 

Also, with a VF-6 machine, is the Rotary table facing up towards the Z axis? If yes, and the RAH is programmable, then you might have a problem, since the two rotary axes would essentially both rotate about the Z-axis. If that is the case, I don't think the Gen Fan 5X will work for this application.

 

The Gen Fan 5X Mill Post would work if your Table Rotary was rotating on X or Y, with the RAH rotating about the Z axis of the spindle. It might work for what you want to do, but you'll have to be especially careful to generate a path that only has a single axis of rotation (for a "live 5" vector-based toolpath).

 

If you are just looking to rotate the RAH into a fixed position (albeit, a programmable one), then the Gen Fan 5X Mill post will probably work ok.

[Rotary Ninja]

It is a fixed 90 degree head. And yes, the rotary is facing vertical rotating about -Z- axis. I will post up an MCX file when I get time to work on it more. It will be a few days before I get back to this part.

 

Thanks for the help!

[guitar]

It is a fixed 90 degree head. And yes, the rotary is facing vertical rotating about -Z- axis. I will post up an MCX file when I get time to work on it more. It will be a few days before I get back to this part.

 

Thanks for the help!

 

I am also working on a part that seems to be identical to your situation. A 3 axis vertical with a rotary indexer lying flat and rotating around Z axis. 6 holes must be drilled and reamed on the id. My RAH will be in the machine with the tool tip facing X+. So, I defined my RAH in MC with a 180deg angle.

The mastercam MPROUTER.pst is setup (sort of) to handle this task. I say sort of, because the post is kind of funky. I am not a router guy, and do not understand why they set some thing up like this. Particularly, the work offset system needed debugging. It kept on overriding the work offset I wanted to be G57 as G55. I got to the bottom of this and fixed it. There were also alot of other things that needed to be changed, and a few for personal preference. WCS was setup as top of part with the T/C planes set to left side.

[guitar]

Here is a problem. This works fine for single axis. But, when you put this on a vertical with a rotary indexer that rotates around Z axis, things do not work out so well. I have ID holes located every 120 degrees (perpendicular to centerline). Pretty simple, huh?Probably 10 minutes to write this by hand. When I try to rotate this, it doesn't work worth xxxx. In fact, it seems to use the "Machine View Angle" in the RAH description as the C-axis rotation angle instead of using the indexer to control rotation around Z-Axis. Quite frankly, the MPROUTER.pst needs alot of work to do anything. The ONLY way I can get this to rotate is to use Transform/rotate, Method "Tool Plane", and output as subprograms. If I don't use subs, I get garbage. And, the clearance position must be The center of rotation. In other words, Absolute zero. Then, on top of this, editing RAH tools is a PITA. You can't just copy/paste. Every tool must have it's own definition in the Machine definition. And, once you describe those RAH, or edit, they do not automatically update the program. You must start over with your tool selection. What a Fkin headache!!!! Hell, this post can't even output sub programs in transform correctly. It doesn't even have code for G28?!? How many more years to MC users have to fight this xxxx? Maybe, by Version XXZ they will finally get this to work. MC needs to stop adding more features until they get the " features" from 10 versions back to work properly.  

[Colin Gilchrist]

Here is a problem. This works fine for single axis. But, when you put this on a vertical with a rotary indexer that rotates around Z axis, things do not work out so well. I have ID holes located every 120 degrees (perpendicular to centerline). Pretty simple, huh?Probably 10 minutes to write this by hand. When I try to rotate this, it doesn't work worth xxxx. In fact, it seems to use the "Machine View Angle" in the RAH description as the C-axis rotation angle instead of using the indexer to control rotation around Z-Axis. Quite frankly, the MPROUTER.pst needs alot of work to do anything. The ONLY way I can get this to rotate is to use Transform/rotate, Method "Tool Plane", and output as subprograms. If I don't use subs, I get garbage. And, the clearance position must be The center of rotation. In other words, Absolute zero. Then, on top of this, editing RAH tools is a PITA. You can't just copy/paste. Every tool must have it's own definition in the Machine definition. And, once you describe those RAH, or edit, they do not automatically update the program. You must start over with your tool selection. What a Fkin headache!!!! Hell, this post can't even output sub programs in transform correctly. It doesn't even have code for G28?!? How many more years to MC users have to fight this xxxx? Maybe, by Version XXZ they will finally get this to work. MC needs to stop adding more features until they get the " features" from 10 versions back to work properly.  

 

Unfortunately, without understanding how the Router posts are setup internally, many people get frustrated because they don't understand what is supported, and what is not supported.

 

The Router posts only support a Rotary Axis in the HEAD. The post is designed to support block drilling, aggregate tools, and RAH attachments, on the head side.

 

Mastercam uses the Tool Plane and WCS mechanism to derive rotary angles inside the post. This is supported through the use of the 'rotaxtyp$' variable, and this, more than any other setting controls how MP derives angular output from the planes.

 

For your application, Router is the wrong post to use in my opinion. The Generic Fanuc 4X Mill Post would do this, but you will have to change the rotary settings internally inside the post itself.

[crazy^millman]

Here is a problem. This works fine for single axis. But, when you put this on a vertical with a rotary indexer that rotates around Z axis, things do not work out so well. I have ID holes located every 120 degrees (perpendicular to centerline). Pretty simple, huh?Probably 10 minutes to write this by hand. When I try to rotate this, it doesn't work worth xxxx. In fact, it seems to use the "Machine View Angle" in the RAH description as the C-axis rotation angle instead of using the indexer to control rotation around Z-Axis. Quite frankly, the MPROUTER.pst needs alot of work to do anything. The ONLY way I can get this to rotate is to use Transform/rotate, Method "Tool Plane", and output as subprograms. If I don't use subs, I get garbage. And, the clearance position must be The center of rotation. In other words, Absolute zero. Then, on top of this, editing RAH tools is a PITA. You can't just copy/paste. Every tool must have it's own definition in the Machine definition. And, once you describe those RAH, or edit, they do not automatically update the program. You must start over with your tool selection. What a Fkin headache!!!! Hell, this post can't even output sub programs in transform correctly. It doesn't even have code for G28?!? How many more years to MC users have to fight this xxxx? Maybe, by Version XXZ they will finally get this to work. MC needs to stop adding more features until they get the " features" from 10 versions back to work properly.  

 

You have stumbled into one of the areas I consider Mastercam the weakest by far with (Well next to ****/****). I normally will define the RAH and hope it work, but unless you are a 100% dedicated post guy that knows MP posts like the back of your hand not easy to do IMHO. I have done my share of it over the yeas and I cannot say I can think of any time since I used it can I say yeah lets do some RAH work in Mastercam. Most times it is okay lets figure this out again. I know shops that do RAH almost every week and are good at it with Mastercam so I am not saying it can't be done, but a good post is Key here. Trying to make one yourself without that very strong MP post background is going to struggle. Again those are my thoughts on it.

[crazy^millman]

Unfortunately, without understanding how the Router posts are setup internally, many people get frustrated because they don't understand what is supported, and what is not supported.

 

The Router posts only support a Rotary Axis in the HEAD. The post is designed to support block drilling, aggregate tools, and RAH attachments, on the head side.

 

Mastercam uses the Tool Plane and WCS mechanism to derive rotary angles inside the post. This is supported through the use of the 'rotaxtyp$' variable, and this, more than any other setting controls how MP derives angular output from the planes.

 

For your application, Router is the wrong post to use in my opinion. The Generic Fanuc 4X Mill Post would do this, but you will have to change the rotary settings internally inside the post itself.

 

Colin that is about everything related to Mastercam 5 Axis posts that come out of the box with Mastercam. We use 3rd Party people for 5 Axis posts just not worth the effort any more to keep trying to figure out what will or will not work.

[guitar]

Colin that is about everything related to Mastercam 5 Axis posts that come out of the box with Mastercam. We use 3rd Party people for 5 Axis posts just not worth the effort any more to keep trying to figure out what will or will not work

 

Realistically, I think this is a marketing scam. Let's make some half xxxx posts so we can screw them for $5000 more once they figure out they can't do with mastercam what they expect. Most of these posts look like they were written by someone that has never seen a g-code program. Everyone of these has to be reworked to some degree. This is version 18 of a software that has been around for 20+ years. Like I said. I could program this by hand in 10 minutes. Why does MC give us such a headache with things like this? Extortion? We also had bought a 5-axis post from MC. We had them rework it 15 times and they still did not get it right. We finally gave up.

[djstedman]

So I guess I should be pretty happy that I was able to modify my 4Axis post for a VMC to include a Alberti Dual angle head and use it to circular interpolate holes simulating a 5th Axis.

 

I was pretty impressed with myself at the time, but really I had no idea others struggled with it so much..

[crazy^millman]

Realistically, I think this is a marketing scam. Let's make some half xxxx posts so we can screw them for $5000 more once they figure out they can't do with mastercam what they expect. Most of these posts look like they were written by someone that has never seen a g-code program. Everyone of these has to be reworked to some degree. This is version 18 of a software that has been around for 20+ years. Like I said. I could program this by hand in 10 minutes. Why does MC give us such a headache with things like this? Extortion? We also had bought a 5-axis post from MC. We had them rework it 15 times and they still did not get it right. We finally gave up.

 

Not sure about that. If it were just marketing then no one would be able to do it. Like I said others do it, but nothing something I have had to do in the last 5 years. I could probably wrap my brain back around it and get it done, but a out of the box ready go thing is not soothing I see. In CNC Software's defense it would be real hard to make a out of the box solution with all the possible heads and way it could be used would be hard to have a does everything solution. I do think a better generic one could be readily available, with better documentation on how a user could modify it to make it suit their needs.

[crazy^millman]

So I guess I should be pretty happy that I was able to modify my 4Axis post for a VMC to include a Alberti Dual angle head and use it to circular interpolate holes simulating a 5th Axis.

 

I was pretty impressed with myself at the time, but really I had no idea others struggled with it so much..

 

Yes you should.

 

Question how did that Right Angle head look in your Verify and Machine Sim?

[djstedman]

Verify worked good showed the tool at the correct angle and in the correct position, don't know about machine simulation since we don't have it setup here.

 

I have wanted to setup machine sim, but Mazak won't give us models without paying and management here won't pay Mazak for the models.  I started making models so I could set it up myself but eventually just scrapped the plan.

 

Honestly I don't think anyone in management here that makes the decisions regarding money has the understanding of machining necessary to make informed decisions - it's why we also don't have Vericut even though we often do full fourth rotary work and proving out programs can often be a 3 hour heart attack.  Gotta love having a part programmed to do profiling in full fourth at 80 or 90 inches a minute that you get to prove out with your hand on the e-stop.

 

But yeah anyhow verify looked exactly as it cut in the machine.

[crazy^millman]

Verify worked good showed the tool at the correct angle and in the correct position, don't know about machine simulation since we don't have it setup here.

 

I have wanted to setup machine sim, but Mazak won't give us models without paying and management here won't pay Mazak for the models.  I started making models so I could set it up myself but eventually just scrapped the plan.

 

Honestly I don't think anyone in management here that makes the decisions regarding money has the understanding of machining necessary to make informed decisions - it's why we also don't have Vericut even though we often do full fourth rotary work and proving out programs can often be a 3 hour heart attack.  Gotta love having a part programmed to do profiling in full fourth at 80 or 90 inches a minute that you get to prove out with your hand on the e-stop.

 

But yeah anyhow verify looked exactly as it cut in the machine.

 

You missed my point. I know the tool will show up just fine in the Backplot and Verify. I am asking about the RAH itself. What I have had to do it extremely tight places is model up the RAH and physically put it in the part with the tool in it to make sure the RAH would clear. That is where I would like to see Mastercam be able to handle RAH. Maybe a pipe dream, but for those doing RAH having the ability to see the head along with the tool would be invaluable IMHO.

 

Yes been there and done that with the Hand on the E-Stop and watching every line of code. Running that Setup part and praying I don't rip the RAH off the machine.

[djstedman]

Yeah totally didn't catch your meaning on the first time through..

 

But yes.. I have thought many times how it would be nice to be able to have items specified as 'non rotating'

 

For instance in our bigger machines we have probes heads that don't rotate at all .. and it would be nice to be able to model them to check clearances..

 

For the job I did with the RAH I modeled the head as a separate item and moved it around the part into all the different positions to verify clearances, have had to do it with other things as well..

 

Hopefully we get that in Mastercam 2099 lol