[aldepoalo]

Hello Everyone!

So this topic has been a hot one while I've been at the westec show, now that I am back I want to address the questions and get you all sorted out...

Here is a short list of topics I will be covering, please add to this list if I miss anything.

1_ ) What are the limitations for roughing with the Rotary Tool Path
2_ ) What is the best practice for roughing parts on your 4th axis
3_ ) What is the base point and what effect does it have on your tool path.
4_ ) Where is the axis of rotation defined and how to you change it
5_ ) Advantages of 4 axis Pro over 4 Axis Standard for off center cutting.


This is the sample part I will be using to demonstrate these topics:

Attachment 205150

[BurrMan]

2.5_) Determine areas, where/how much material is left from the rough, to define/design a good finish cut

[magicniner]

Al,
If I'm best roughing my beavertail with an indexed 3-Axis strategy I'm happy with that, I'd given up on generating any roughing passes fairly early on and was just trying for a rotary finishing pass that followed the surface, would you mind adding -

2.2_ ) What are the limitations for finishing relatively thin, non-round, significantly off centre parts with the Rotary Tool Path
2.4_ ) What is the best practice for finishing relatively thin, non-round, significantly off centre parts on your 4th axis

Regards & Thanks,
Nick

[BurrMan]

Al,
If I'm best roughing my beavertail with an indexed 3-Axis strategy I'm happy with that, I'd given up on generating any roughing passes fairly early on

The step down in the rotary is for easing the finish into the cut because you cant get an exact "stock leftover" using index roughing. You cant/shouldnt rough with rotary.

[rckdef]

Hi Al-
Before you get started i would like to take this time
to Thank you again for your effort in getting me
going with the 4-th Axis. I finally got running again
and took the time to run a test on 4 Ax imdexing
and also 4 Ax rotary--am pleased to report after all
the difficulty we had with V3 simulation and post processors
your help and choices were right on--i can now Index
or rotary including simulation--Thanks Again--Good Job**
RICK

[aldepoalo]

What I think many of you were under the impression that the rotary tool path would be trimmed to the stock... That is not the case and is the reason why this tool path is not intended for roughing. Just like burr said it's to "ease" the finish pass by taking multiple depths.

In the 4 axis pro tool path you could use morph between 2 curves and trim the tool path to the stock, I'll get into this in more detail with in future posts....


Here is a screen shot of the trimmed tool path created with

Attachment 205178

[aldepoalo]

Let's just get started.

Attachment 205202

I think this is where there is a lot of confusion about the rotary tool path. I mean come on now it even says "Roughing Passes" So I can't blame you for wanting to use this tool path to rough your parts from bar stock. The roughing passes are " offset" from the part geometry by the spacing your set and the the number you define.

Attachment 205204

What this is doing is starting with you finish geometry and offsetting out by the increment and number of passes you setup. Completely different from your 3D tool paths that start at your stock and steps down at your DOC till it gets to your part geometry.

So with rotary roughing it's only intended for semi finishing.


In this example I can't seem to generate more the 3 passes at a .25" increment. I am not sure if this is something hard coded into the program or not, this is also why in the other thread you've seen users creating multiple rotary tool paths to "create" the additional passes that were wanted.

Attachment 205206


For some samples you maybe be able to use rotary roughing passes if the finish part is close in shape to the bar stock,but for many it will not. Especially those are have off center cutting. The rotary tool path roughing doesn't look at your stock geometry and isn't designed to do so.

The best practice for roughing your parts on a 4th axis is to index 3D rough, index 3D rough. Then use the rotary roughing to semi finish, and then the rotary for finish which I'll get into more detail in this thread.

[RAF.]

7- How to leave a clean up allowance for the round journals in the 3D index roughing and not get the rapid crashes on the sides of the counter weights when using 4th axis Rotary for journal finishing with out using multiple steps with the step limitations. If we had selectable X,Y and Z allowance there would be no problem. We could leave just the YZ allowance and finish in one pass in Rotary Feature. Or is the solution to Draw oversized journals for 3D indexing roughing?

RAF

[ShortTrack]

Al;

RCKDEF is spot on - thanks tons for your help.

A verbal description of what "Point Tool to Rotary Axis" is, and also "Gradual Machining Angle XY Change" mean would be great.

BTW, I have found you can successfully have over 10 passes in some cases. Yes, they start at the finished geometry and work out ....

No hurry here.

Thanks again,
-STrack

[aldepoalo]

I agree there are a few options that I need to clear up myself. The rotary tool path is truly a 5 axis tool path that in the back round options have been defaulted and an interface was created just with the options needed for 4 axis rotary. So I will be going over all the options and features 1 at time.

[aldepoalo]

4 axis cutting is slower than 3 Axis cutting. If and when you can get away with cutting in 3 axis do so! For the sample part we are working on using an index, 3D rough, index, 3D rough is a good method to remove material quickly get the part ready for the rotary tool paths.

This video shows the steps to setup your index systems, create your roughing tool path, and simulate your work.

[aldepoalo]

When it comes to your rotary tool path you have the ability to adjust your base point. By default your base point is based on you machine setup location. The base point is the "center line" of the rotary tool path that will be created.


Attachment 205390



Attachment 205392


In the above example the tool is running along the part as it should be. This is because base point or "center line " of the rotary tool path are correctly aligned with the part. By default your base point values are X0 Y0 Z0, so if you machine setup is located where the "center line" of the rotary tool pah should be, there is no need to make any adjustments.

Now let's take a look at an example where you need to make an adjustment to the base point.

Attachment 205526


Attachment 205396

In this example the machine setup is at the top of the part and the base point settings are the default. You can see the tool path "center line" is now located at the top of the part and the tool path is incorrect.

So how do you fix this? It's easy adjust your base point.... The value you define as you base point is what allows you to "shift" the "center line" of your rotary tool path. For this example we would need to measure the distance from the machine setup to where we want to define the "center line" of the rotary tool path. We measure and input this value in the base point.

Attachment 205398

Attachment 205400

* Notice the Z value is a negative, this is because we are moving the "center line" of our rotary tool path down by 1.25" from our machine setup location.

Now recompute your tool path....


Attachment 205402

Now you can see by making the adjustment of the base point, you have the correct tool path to follow this shape.

At this point you should have a better understanding about what the base point is used for and how to use it on your parts.

[aldepoalo]

Lets look at how you can control where the tool path starts and where the tool path ends.

Attachment 205528

You have this option under the parameters tab, and you use these values to control where the tool path starts and stops. These values are based off your machine setup.

Attachment 205530

Attachment 205532


Now if my machine setup was located in the middle of the part the tool path would look like this, using the same start stop settings.

[aldepoalo]

Using the concepts we've learned so far the next video will be how to apply the rotary tool path to the Rod journal which is off center from the main journal

[aldepoalo]

Here is a screen shot of the simulation

[aldepoalo]

So here is the next video showing what we have learned so far. More still to come...

[aldepoalo]

What is this feature and what effect does it have on your tool path?

Attachment 205694


This feature is used to control the " tilt" of the tool... It will only come into play when you are using a side shift value.

Attachment 205700

In the above example we have a rotary tool path with no side shift.

Attachment 205702

In the above example we have a rotary tool path with a 1" side shift.


You can see how the tools tilt or orientation is parallel with Z . Now let's take a look at what effect the "point tool to rotary axis " will have on this tool path.


Attachment 205706

You can see how now the tool tilt or orientation is pointed to the rotary axis / " center line" of the rotary tool path.

So what does it all mean?

It will have an effect on what "edge" of the tool is being driven along your surfaces. By using the side shift value you can have the tool path use the "side" of your cutter or more of the side of your cutter base on the side shift amount.....

I hope this clears use what this option does and how you can use it.

[aldepoalo]

Tool Engagement with 1" side shift

Attachment 205710


Tool Engagement with point tool to rotary axis

Attachment 205712


These sim screen shots show how when using a side shift and point tool to rotary axis, the side shift effect get's canceled out... So why use this option. Well in most cases you would not use this option. There are special scenario's when you have a 5th axis tilt to the part where this option is needed.

[magicniner]

Al,
That's a really neat formalisation of BurrMan's responses to the original thread with some useful additional detail and information.
I'm really looking forward to your coverage of the problems that no one has yet been able to resolve, I'm manually machining a batch of the beavertails next week :-(
Regards,
Nick

[BurrMan]

Al,
I'm really looking forward to your coverage of the problems that no one has yet been able to resolve, I'm manually machining a batch of the beavertails next week :-(
Regards,
Nick

Hey Nick,
Your questions have been addressed and all the answers given. THere's nothing "unresolved"....

One of the things you might have missed is that what you are looking at, while "can be done" on the 4th axis (And has been explained how) is that it is really a "5th axis toolpath" that you are looking at. Here's a video which shows pretty much what you are seeing, and also will show it go into 5th axis where it needs to (Looks really like your beavertail)

NTX2000????????????? - YouTube

You can zip ahead to 1:12 of the video to see the 4th, then look at where it needsa to switch to 5th to cut the part "correctly".

We can get this done in the 4th though. If you are still having issues with the axis non-continuity, you should get in touch with Al, who can log onto your computer with you and help get a clean toolpath on the beavertail, for next weeks cut.