[azam1959]

I do not want to hijack kvom thread on fourth axis ....

I am good with cad/cam for 3 axis. Used various SWs but for now settled with Autocad Inventor HSM for most of the work. When I need carving, I go back to my old friend Vectric Aspire. I am able to use both the SW in single project ....

Coming to the point, I am about to install fourth axis. I am aware of wrapper support in Aspire and played with Inventor HSM as well but got little confused by the g code generated by HSM. In the worst case I will learn by trial and error but I am looking for folks who have successfully programed 4th axis via cad/cam. Perhaps I can get some jump start ....

I was debating about posting this request in the cad/cam forum .... that will be my next stop if I do not get any input here. Just need little help to get going ...

thx

Regards,

[kvom]

The main thing to understand with wrapper code is that it cannot contain any G2 or G3 words. Any arcs need to be replaced by short line segments, so that they are generated as sequences of short G1 codes. CAM programs should be able to convert arcs to line segments. Then the wrapper can convert the Y coordinates to A coordinates as long as the diameter of the work is specified. We are basically talking about engraving on a cylinder.

[azam1959]

and reason for not able to use g2 and g3 is because wrapper is not really four axis .... means we cannot rotate and cut at the same time, right? my hope is that inventor hsm can do better but not sure yet.

reason why i am inclined to use cam is because user do not have to worry about all these details. program ask for dia, center, length etc. etc. and sw simulation is extra bonus.

cheers

[kvom]

The reason arcs can't be interpolated is that the A axis moves are in degrees, not inches or mm. Since your DXF drawing has Y in inches or mm, the CAM program can't translate that into degrees without knowing the radius. And finally, Mach3 wouldn't understand G2/G3 with an A axis parameter either.

CNC wrapping is not a very complicated operation. This program costs $25 and does what you want: CNCWrapper - Home Page

The only additional thing you have to do in CAM is convert arcs to line segments.

Inventor may be able to do what you want, but if so under the covers that's what it is doing.

[AUSTINMACHINING]

In the Inventor HSM post processor, you can un check the box for arcs and it will create line segment moves.

[azam1959]

In the Inventor HSM post processor, you can un check the box for arcs and it will create line segment moves.

after spending hours on swarf and multi axis contour on inventor hsm i am giving up for now ... in the help file i saw support for four axis/indexer but it is missing in the actual sw. hope better 4 axis support is on its way ... so in the mean time I am back to vectric aspire. Wrapping post processor create g1 code; these are two sample lines from the file generated by vectric aspire
.....
N230 G1 X5.0000 A0.0000 Z0.7100 F50.0
N240 G1 X5.0000 A-4.2857 Z0.7100
.....
f50 in line 230 is coming from tool data base where I set linear speed.
Issue is in line 240 A axis move very slow because of G1.
Manually issuing G0 Axyz move A axis at reasonable speed.

I am not ready to tweak post processor yet and google search did not yield any insight. I am sure I am not the first person who has this issue .... so any idea how to get aspire mach3 wrapping post processor to generate G0 code for A moves?

cheers

[kvom]

after spending hours on swarf and multi axis contour on inventor hsm i am giving up for now ... in the help file i saw support for four axis/indexer but it is missing in the actual sw. hope better 4 axis support is on its way ... so in the mean time I am back to vectric aspire. Wrapping post processor create g1 code; these are two sample lines from the file generated by vectric aspire
.....
N230 G1 X5.0000 A0.0000 Z0.7100 F50.0
N240 G1 X5.0000 A-4.2857 Z0.7100
.....
f50 in line 230 is coming from tool data base where I set linear speed.
Issue is in line 240 A axis move very slow because of G1.
Manually issuing G0 Axyz move A axis at reasonable speed.

I am not ready to tweak post processor yet and google search did not yield any insight. I am sure I am not the first person who has this issue .... so any idea how to get aspire mach3 wrapping post processor to generate G0 code for A moves?

cheers

Increase motor speed in mach3.

[azam1959]

I thought motor speed will impact only G0 and not G1. I will give this a shot along with acceleration.
thanks Kvom

[azam1959]

issue was neither velocity nor acceleration. there is a setting to use radius for feed and since my centerline was coinciding with rotational axis i kept this value zero. changing this value to correct radius did the trick. i think i can use this setting to increase the speed as well ... folks who are using aspire, one anomaly for carving on cylinder .... centerline is at rotational axis but carving start at 0 and not at surface/radius ... carving tool is zeroed at centerline though.

at this point i am up and walking .... enough to get going. here is the video of my first, well second cut; i cut cylinder from square and then carve some arabic calligraphy. will stain and keep it as souvenir but please understand that this is packing wood not suited for carving ....

https://youtu.be/BJqglHXwz90

i am again taking the risk of posting a picture. appologies if photo is not sideways or upside down ...
Attachment 282804

Thanks for all the folks who helped me on this thread as well as on Kvom's thread. Person who advised me on how to remove the rust, I order chemical from amazon and will follow through as soon as i get it.

Guess I can go on hibernation for coupe of years till I get fifth axis hardware :-)
Regards