How to set limits for continuous 5 axis machining

[iamcdn79]

This is my first attempt at creating a continuous 5 axis machining toolpath. I need some input into how I can set limits on my C axis so it doesn't hit the table. In the attached video when the C-Axis goes to +180 it will hit the table. How can I make the safe area between C -90 and +90?

I've tried changing the tool axis limits and also creating a polygon window using the update within region option to no avail. 

I don't know if this is possible or not.

[iamcdn79]

Attached video shows how I tried changing the C-Axis limits for a particular region but it did not work

[5axes]

With the sample part ( just the surfaces used for the toolpath) it would be more aesy to give you an answer. I'm trying to reproduce your problem but without your parameter and the geometry of the head it's not easy.

Regards,

[iamcdn79]

@5axes attached is the project.

It seems the problem lies when my cutting direction is set to zig zag for the constant z toolpath (toolpath 1_1). When it is set to climb (toolpath 1) the C-axis seems not to go to C+180.

[rob_carri]

How have you uploaded the video? And I passed you a video

[rob_carri · Accepted solution]

Hello

I see you've used avoiding auto collision.

When you take time with 5 axes you will see that it is more like using patterns, directions or lines to control your movements.

I have created a pattern of the top edge of the closure, and I have told the strawberry to follow that pattern from the line.

I have gone to the orientation vectors, and as it is logical there you set in which angle you want to start working, she will look for the easiest angle depending on the movement that your head can do, watch the video

see video here       http://es.tinypic.com/player.php?v=rszajd&s=9#.WMA1LVXhBhE

[iamcdn79]

@rob_carri Yes there are 2 videos uploaded already, can you not see them? 

What do you mean you passed me a video?

[rob_carri]

@iamcdn79

Sabia CÓMO subir vídeos, busqué Un sitio web Donde párrafo Acoger uno

Lee Mi Mensaje anterior to see Si Es La Solución Que busca

[iamcdn79]

@rob_carri I did what your snapshots are showing. Created a pattern, Selected 'From curve' for tool axis and selected the pattern I made, changed my machine axis control to 'Direction of travel' but the result is an uncalculated toolpath.

Attached is the project

[rob_carri]

@iamcdn79,

did you see the video?

[iamcdn79]

Yes I clicked on the link but there aren't any powermill videos shown

[rob_carri]

Put this address in the explorer bar       http://es.tinypic.com/player.php?v=rszajd&s=9#.WMA8BFXhBhG

You have the pattern very down.

If you want to leave the pattern down you have to choose towards the curve

But towards the curve is not the correct solution, because the tip of the tool will look towards it and do not lower the path giving you collision.

Create the pattern above ....

Wait i do it to you

[5axes · Accepted solution]

On a simple program like this one Usualy you can solved your problem with the "Smoothing option"

Try these settings on your program 1_1

I have set 45° on the Azimuth angle to get the minimum C movement but more than the Correction angle it seems to be the "Smoothing distance" which have an influence on the result. I'm a "Metric User" so I'm not very  familiar with the parameters in Imperial system. 10 was something correct in my mind according to the size of the milled geometry.

[rob_carri]

Veo Que El movimiento de la Máquina sin configurado Está Bien

El eje que hace? Girar la Cabeza ez C y en el Proyecto gira Y, no entiendo

I'll give you a project tomorrow and see it

[jonathan.artiss · Accepted solution]

Hi @iamcdn79

Have a look at this video http://autode.sk/2mmkZ2B

I'm not sure that you actually need tool axis limits set, you just need to know how to flip the machine tool around. 


​Cheers,

[iamcdn79]

Thanks @5axes How do you know that an azimuth angle of 10  will get the C axis movements between -90 and 90. I originally had it set at 5, is there some kind of chart to reference to?

[iamcdn79]

Thanks @rob_carri when I raise the pattern up it does now give me a calculated toolpath

[iamcdn79]

Thanks @jonathan.artiss I will play around with those settings now that I see what they can actually do

[5axes]

---

iamcdn79 a écrit :

Thanks @5axes How do you know that an azimuth angle of 10  will get the C axis movements between -90 and 90. I originally had it set at 5, is there some kind of chart to reference to?

---

 In this case  it's not the Smoothing angle the most important ( 5 is also correct)  that's the distance which make the difference.  I'm using 10 ( again because your part is in Inch) .   You are trying to make an automatic 5 axis collision advoidance toolpath in this case the orientation of the tool / the geometry is not very important so I'm always try to use a large value for this tolerance to see if there is a difference nothing really exact just 45° and 250mm for example. If it's works i'm happy if not I'm trying to use  an other solution 🙂 one of the solution given by @jonathan.artiss but I'm also try to always minimize 5 axis movement. I will give you the secret of a good 5 axis toolpath : 

A good 5 axis toolpath is when you can do it just with 3 axis 🙂

[iamcdn79]

@jonathan.artiss when you changed your azimuth angle to 180 in the machine axis control that required a recalculation of the toolpath.

Is there a way it would work by not having to recalculate the toolpath?

When I access the dynamic machine control and select 'Swap machine tool configuration" and click 'Update Toolpath' it wouldn't require a recalculation for a 3+2 toolpath.

I can click on 'Swap machine tool configuration' but the 'Update Toolpath' icon is grayed out for the toolpath you created.