DMU50 + ITNC530 5 Axis Problems

[keithZ5MNA]

Hi All, 

I have been using fusion for a bit on 3 Axis and it's working out pretty well on my old Haas and new Doosan.  I thought I might try the 5 axis package out and have run into a number of problems.  

I have a 2011 DMU50 using a ITNC530 controller.  There is a post available on the website for this so I thought I might be ok.  

I am trying to contour on some curved lines I created on an imported model to clear away a leftover radius formed by the preceding 3 axis cycle. 

1. The machine "jolts" when moving along the contour, it goes smoothly for a second and then stutters with fast, small movements and then smooth again.  I have changed the tolerance from 0.01 to 0.15 but it still happens.  

2. The Z plane return outputs as Z+0 rather than Z-1 (also the x should be -500 and Y-1  but they are both +0 as well)

3. The Z axis is 50mm higher than it should be. 

I have been using Hypermill previously and if I go back to that everything is fine so I am pretty sure it's a post issue.

Any ideas?

Also would be interested in paying for a post for the machine too, I can see myself using it more if I can get it to work.

[a.laasW8M6T]

Hi

The jerky motion is likely due to Smoothing not being turned on(in post properties), which means Cycle32 doesn't get activated

The Z retract can be handled 2 ways.

1st you can select "Use M140" , this will do a full retract in the tool axis, but will not do a Z retract at the very start of a program because no tool axis has been defined in a tool call yet.

Otherwise you can leave "M140" unchecked and you will in both case need to go into the post and find the section for the home positions, uncomment them and enter the correct values (M91)

 

[keithZ5MNA]

Hi, thanks for the help.  I had some success with the smoothing.  

I needed to change it to 0.2 on the processor and 0.2 within the program itself.  It's still not fluid however like I would get on Hypermill. 

The home position alteration did not work, it inputs another value altogether than the one I had altered the post with.   Using M140 gives me an error.

The Z is still too high, I am wondering if it is reading the correct work offset to be honest, there seems to be no place to change it (unlike changing G54 - G55 in the Fanuc post)

[a.laasW8M6T]

Ok,

Can you share your post processor here so I can have a look?

The toolpath setting can affect how it runs on the machine too.

try reducing the segment length and sweep angle to like 0.5mm/0.5 deg

For your work offsets, if you have 0 in the field the post will not output cycle def 247, so will use what ever is the active preset, you need to use 1 and up in the WCS field 

[keithZ5MNA]

Sorry, late reply.  Thanks again for your help.  

I have been playing around with the setting and it looks like the one that helped the most was in the "linking" - High feedrate mode and "always use high speed".  I think the smoothing also assited and I have added a value to the fanning too.

There was an official tutorial for engraving which said doing this will help in 5 axis movement and it does make the movements more consistent.

I still have an issue with incorrect home position naming however.  I was using the standard ITNC 530 post from the website - https://cam.autodesk.com/posts/post.php?name=heidenhain

[a.laasW8M6T]

Hi,

Sorry I pointed to the wrong place in the post to edit, they have changed slightly to the one i'm using.

Try this one