5 axis trunnion issues

Greetings from Argentina! A few months ago I began working in a mold making shop that has recently acquired a big 5 axis mill (Y=10m, X=5m, Z=2.5m) and we have more or less got it running and this forum has been tremendously helpful.

I am a naval architect with have little to no experience in CNC machining, however after some months of trial and error I have learned a lot, but some solutions I have come up with empirically may not be the most efficient way to use the machine and I now turn to you hoping to tidy up our work process. This is my first post

The machine has a Sinumerik 840D controller, and I program in Rhinocam. So far it has worked, but the post processor file was more or less concocted by the previous guy with some help from the machine provider and a few little additions of mine. It is far from perfect and I don´t understand most of it. Also the Sinumerik controller was never properly set up by a professional. The machine builder sent a programmer a few times and he was really helpful for setting up some parameters, but I believe there is a lot more to tweak. Aside from this machine, we have 2 small 3-axis mills, one of them with Syntec and the other uses Mach3.

What follows is part of an endles list of doubts so please bear with me and if anyone can help me with at least one of them I will consider this a success. Most of them are about Rhinocam and a few about the machine itself

1- When programming for the 3-axis machines, Rhino lets me place the Zero point wherever I want. But as soon as the machine specification is set to 5-axis, it always uses the cPlanes "origin" as Zero point and there is nothing I can do to change it. Is this normal in RhinoCam? (or in 5-axis programming for that matter)

2- I was only able to program very few 5-axis operations. Mostly I index the rotary axes and use it in 3+2. This is due to the fact that in 90% of the surfaces I have to machine, RhinoCam doesn´t generate a good toolpath. It may be because of the way they are trimmed or mirrored. Below are some examples.
Notice how it sometimes responds well to one surface but not to its mirrored "twin". And also it´s not always the same side that brings problems. I tried deleting and mirroring again, flipping normals, etc. to no avail. So far the only thing that worked is using MIRROR function in the gcode (which mirrors XYZ axes) AND changing the machine axes definition in RhinoCam from "+Z, -Y" to "-Z, +Y" which mirrors the rotary axes. This brings me to my next point...

3- There is no machine definition that allows for a straightforward programming of the machine. "+Z, -Y" Outputs a code that succesfully moves the machine in simultaneous 5-axis mode (that is on the few ocassions when I can produce a toolpath), However if I want to machine in 3+2 mode, I need to change it to "-Z, +Y". I believe this to be a symptom of a deeper problem involving the patched up postprocessor file.

4- There is another "glitch" that scares me from using simultaneous 5-axis in general. When the trunnion vertical rotary axis B reaches it´s software limit in the middle of an operation, it has to rotate all the way around in order to continue machining. When this happens the tool only moves a very little bit away from the piece, which is never enough to avoid collision. So far this only happened in tests machining styrofoam so the machine is ok. But I have not found any parameter in the controller or in Rhino to change how much the tool moves away when this happens, or in what direction. I have avoided collisions by extending the range of motion of the B axis and personally checking the code in places where I know it may reach the limit. This is very tedious and inefficient

5- Bonus question; I have not found a way to use the machine in "4-axis" mode, since rhino seems to interpret 4 axis operations as only suitable to rotary table machines, or lathes. Is this so, or am I missing something?

Hi,
there are broadly two types of simultaneous five axis toolpaths.

The old school way was that the part has to be drawn in your CAM software with the part (and toolpath) origin drawn at the same location as the machine centre.

For instance if you clamp a block of material in a self centering vice such that the centre of rotation is one inch below the bottom of the material.....then your toolpath
must also be centered on that location. This means that unlike a three axis toolpath where you can 'zero' the machine to any given point.on the part, with five axis the
part has to be placed relative to the machine center.

Most modern 5 axis machines are better than that. The motion controller will allow you to set the part zero wherever you like but then internally recalculates everything to
accommodate the the machine centre of rotation is displaced relative to your part. This requires '5 axis kinematics'. I would have thought an 840 was capable of that, but may require
a special license over and above what you have. It also requires a post processor that leaves the data in such a manner that the machine control can do its thing.

Obviously be able to set the part zero at will with a five axis machine is very desireable......but is limited to those machines which are designed for and enabled to do it,
usually very expensive and modern machines..

From your description I do not think your machine is set up like that.

I have just finished building a trunnion fifth axis for my machine. My CNC software/controller (Mach4) does not have kinematics so I am perforce required to use the older
method. This method is less convenient......but funnily enough a bit easier to understand. I happen to know for instance that the machine centre is 22.5mm above
the fifth axis platter, and I place the raw material in relation to that.

In the months or years perhaps to come I would like to write my own kinematics module, but at this time I am still exploring and coming to understand the earlier, tried and trued
method of running five axis toolpaths.

I use Fusion 360. In order to do simultaneous five axis toolpaths I have to buy Fusion Machining Extensions at another $2200NZD/year, as that allows genuine five axis toolpaths.
It may be the Rhinocam cannot do simultaneous five axis, but may be able to do 3+2. It is quite common for a CAM solution to do say 3 or 3+1, or simultaneous 4 axis, or
3+2, but full simultaneous five axis is usually a cut above....and costs a bloody fortune!!!

You need to do a bit of research and find out what your machine is capable of, and also whether your version of Rhinocam has a full simultaneous five axis license.

Craig

I've only used Rhinocam in 3 axis mode,but have done more 5 axis with Mastercam in the past.The business of refining a 5 axis post processor is not an easy one and we had a specialist write one which wasn't inexpensive but the result was tht we had zero problems.From the report above it seems like there is a parameter in the post that needs to be given a different numeric value so that the retract distance is greater than the distance from the pivot point to the tool tip.One other thing to watch out for is the manner in which the distance from the pivot point of the head to the tool tip is compensated for with varying tool lengths.How have you been doing this?

I don't fully understand how you are setting up the part datum location relative to machine home.I know that it can take a lot of searching to find a "rogue" normal and flip it and would ask you to consider how difficult it might be to convert your selection of surfaces to a solid.

Using simultaneous 5 axis cutting can be the fastest way to arrive at a finished surface but do be careful as the motor body or the casting it hags from can contact the surface of the job-with disastrous results.The same can happen with any other cutting technique and you may need to resort to using machining boundaries,drawn on a separate layer of Rhino,to limit the area being worked on.Clearly you ought to use the same orientation as the toolplane when doing the drawing.

I wouldn't know how to use Rhinocam in 4 axis mode but in Mastercam it is possible to lock one of the rotary axes and use the other 4.Most 4 axis work is done with a 4th axis parallel to the table of the machine,similar to a lathe and it seems your setup assumes such machine configuration.

One final question,do you record a G54 value for the job or use datum blocks?I mention this because I used to work in a remote location where the power sometimes cut out and without some reference it was hard to re-establish the location of a job when it came back.Similarly it was useful to note the line number of the job every once in a while so that a chunk of the program could be edited out to avoid redoing an area.

- - - Updated - - -

I

Have you asked Mecsoft about any of these issues? Usually, their tech support is pretty responsive, and they will write (or re-write) a post that matches the kinematics of your machine, assuming you've got a current 5-axis version of the program.

Quote:

---

Originally Posted by joeavaerage

The old school way was that the part has to be drawn in your CAM software with the part (and toolpath) origin drawn at the same location as the machine centre.

---

This would explain why the Zero point is always forced back to the origin, altought I already filled up the machine specification and it is a head-head configuration, maybe there is some other setting in the postprocessor that I am missing

Quote:

---

Originally Posted by routalot

I've only used Rhinocam in 3 axis mode,but have done more 5 axis with Mastercam in the past.The business of refining a 5 axis post processor is not an easy one and we had a specialist write one which wasn't inexpensive but the result was tht we had zero problems.From the report above it seems like there is a parameter in the post that needs to be given a different numeric value so that the retract distance is greater than the distance from the pivot point to the tool tip.One other thing to watch out for is the manner in which the distance from the pivot point of the head to the tool tip is compensated for with varying tool lengths.How have you been doing this?

I don't fully understand how you are setting up the part datum location relative to machine home.I know that it can take a lot of searching to find a "rogue" normal and flip it and would ask you to consider how difficult it might be to convert your selection of surfaces to a solid.

---

I think the option of hiring an specialist was ruled out as we are on a very tight budget. There was talk of buying Mastercam at some point but since the machine is already running (kind of) and we have some other axis alignment issues which I havent said anything about.. the money is probably going somewhere else at this point.

We do compensate pivot distance and tool length and it is working as expected. since there is no tool changer or gauge sensor what we use is a simple piece of paper to measure the distance from the front of the spindle to the tip of the tool, touching both against a firm surface and substracting the Z values. And for pivot distance, we measured using the classic method of dial indicator touching the face of the spindle and then rotating it 90° and measuring again, subtracting the values and whichever diameter compensation was necessary.

Interestingly enough the 5 axis toolpath problem doesn´t seem to be related to surface normal, since flipping it would give the same (erroneous) toolpath but with the tool machining the "inside" of the model, if I am expaining myself. I will try however what happens if I turn the model into a solid

And yes, we do use work offsets (G54, G55, etc) from the very beginning since we always had several parts in the work area and it became evident we needed to record ther relative zeroes.

Thanks to everyone for your replies. I will keep you briefed on any news

I agree with Andrew's suggestion to contact MecSoft. They are very helpful. You will have better success getting this figured out using their support than a bunch of random suggestions on a forum. Also, the idea of being on a tight budget needs to get tossed out. It's going to cost a lot more to repair your machine than to pay for a good post.

I thought this thread had faded away.I would suggest that one fix might be to look for the retract sequences in the program that accompany the unwinding of the C axis and use Wordpad or similar to edit them such that the A or B axis returns to zero after a retract move and before the unwinding and then returns to the programmed angle after the unwinding is complete.I see that the OP mentions axis alignment issues and with so many factors on a 5 axis machine,it can take a lot of work to get these correct.It is imperative that the centre of rotation of the fifth axis is located exactly coaxial with the fourth axis and that the home position of both rotary axes are precisely parallel with the orthogonal axes.You also need the tool centre to be truly central.