Z Height Off Over 2"

[taylorX5GHV]

Hello, I am new to Fusion and recently purchased a new to me DMS 5-axis CNC.  I am learning both the software and machine at the same time.  I am coming from an AVID CNC with Mach 3/Vcarve.  

I have been able to get the machine and software working together pretty successfully except for one detail.  The Z axis is almost always off.  I say almost because on my 6" long bit it is pretty close to where I want it, but when I switch to a spoilboard bit, which I use more often, it is over 2" too low.

Bear in mind that I purchased two sets of tool holders, and they are different in length.  I have dimensioned the toolholders and paired them to the appropriate bits but I still have this frustrating issue, which requires me to artificially raise the z0 location in order to mill a part. 

I have an automatic tool changer, but no automatic tool probe.  Per the machine instructions I zero the nose of the spindle to the spoilboard surface, then zero the tip of the bit to obtain the tool length which is then input to the tool offset menu.

Any ideas?

@paul.clauss 

[Shannon_IMD]

Can we just clarify this process a little?

1. So you touch off the spindle nose to the job. Do you then set this Z position in the work offset table e.g G54? There will be a calibrate or teach etc.

2. Now you change to the tool you want to set. Bring tool into the same Z position as you did the spindle nose. Now go to the tool offset page and measure or calibrate etc. the Z value into the correct offset number to match the tool number. The value in the tool offset table should match the distance from the spindle nose to the end of the tool as you have just measured the length of that tool in the controller. You check this roughly with a tape measure.

3. You should now be good to go as long as you have used the same work offset number e.g G54 in the setup in your program. The tool length offset number for your tool must be the same as the one you set the tool to in the tool offset page. Also the position of the coordinate system in the setup on the model in manufacture matches the reference you set the work offset on the machine. So the setup coordinate system must be on the top of the model or stock in your model that you used on the actual material on the machine.

Lets start there. There are some nuances to different controls that could alter the result here.

[leo.castellon]

I see that you made another post with the same problem, this can cause confusion. In your other post, you mentioned that your machine has a Fagor controller. Looking through the G code that you posted, I don't see a tool length call out. According to the Fagor manual, this should be called out with a G43, which would be like most other CNC machines: 

Perhaps you could send DMS an email with your g code and explain the problem and see what they say? I am not familiar with your machine nor controller, so I am not an expert on them, but I have been around CNC machines a long time.

LeoC

[Shannon_IMD]

No G43 would definitely do it. Is there a reason you didn't start with the standard Fusion Fagor 8055 post? This post has the G43 in it. You could cover off a lot of the post setup by correctly configuring a machine setup for your tilting head machine.

[taylorX5GHV]

Thank you for the response!

I believe I tried the standard 8055 post when I was first started using the machine and it is not configured for 5 axis cnc's removing a lot of the functionality for me.  The gcode I attached earlier is specifically for tilting the head, so unless I am wrong about the above (Can anyone confirm this?) I am stuck with the post that I have unless I pay a few grand to have someone customize it.  The post I am using came from Autodesk's own Pier9 5axis DMS cnc so I thought it would be a really nice and compatible match.

In regard to G43, when G48 is active (tool Center Point) g43, g53-g59, g92 are all deactivated, see attached from the manual.

I feel I will have more luck here than with DMS because they are likely to blame the software just as the software folks are to blame the machine, but I could be wrong.  I am learning 😄

[taylorX5GHV]

Thank you, Shannon, for your thorough response!!!

Here is my process, which is based on the manual and the tech that helped me set it up:

1. Touch spindle nose to dial caliper until it zeroes.  Notate the length or use g54 to zero the z axis.

2. Install tool and repeat, zeroing the tool to the caliper until it zeroes.  Notate the new length and calculate the difference.

3.  Go into Fagor and select Tables>Tool Offsets>Find an unused D Value(Tool Offset)>Modify Length to the difference between steps 1 & 2 above (Positive Value)

4. Tables>Tool>Define T (Tool Number) to match D (Tool Offset).  Example: T6 = D6, T3=D3, etc.

Now I go into Fusion360 and do the following:
1.  Tool Library>New Tool>Cutter (Input dimensions)>Holder (Input Dimensions)>Accept

I've attached a few screenshots for you to look at.

Thanks again for your help!

[taylorX5GHV]

Hey Shannon,

It has been a while since I tried the standard 8055 post so I ran it again and received an error message on my Fagor controller while trying to run the program, see attached.

[taylorX5GHV]

EDIT:

I thought I fixed it with the below, but there were a few issues:

1: The B axis needs to be rotated, not the A axis, A does not exist.

2: The C axis also needs to be rotated, and the post simply has C at 0.

Based on this, I feel the best solution is to use the Pier 9 DMS 5 axis Post and somehow disable g48, and simply use g43.  What do you think?

-----------

ORIGINAL REPLY:

Ok ,I see what happened, the post defines an A axis but my machine simply has xyz B and C.  I modified the post from A to B and it worked. 

However, I still have the bit about 4" or so too high.

[Shannon_IMD]

There’s some more info in this post

https://forums.autodesk.com/t5/hsm-post-processor-forum/fusion-360-5-axis-fagor-8055-post/td-p/70418...

it looks to me like you need to spend the time in your machine configuration file. Setup your machine in the machine builder. Make sure your linear axis and rotations axis all match what you actually have on the machine. The post will adapt to your machine configuration file. 

[taylorX5GHV]

Ok, some progress here:

There was a Z offset in my zero offsets menu for G58.  I deleted it.

Problem now is Fusion is sending the offset to my machine and my machine is then doubling it.  I deleted the tool offset in my machine and maintained the fusion offset and it zeroed perfectly.  I am not sure if this is the solution as it may lead to issues elsewhere??

Please let me know your thoughts regarding the attached text from the manual.

[Shannon_IMD]

Great to make progress. My understanding is the software is using the tool length from your fusion tool page. So the gauge length there needs to match the tool assembly you load into the machine. If you have slight variations in the tool length between tools then one of the gauge lengths is probably out a bit. You can use the machine and a gauge block to accurately measure the tool lengths. Just zero position screen on spindle nose, then measure each tool. Enter lengths into tool page in fusion. 

The machine pivot point length is the other contributing factor here. So you either enter it into the machine control or into the machine configuration. It sounds like you have that sorted now. Some test cutting with head at 90 and 270 degrees will let you know if you’ve got that length right. Machine a rib from each side. If your tool length is right in the tool library, then keep adjusting the pivot point until the rib measures the expected width. 

[taylorX5GHV]

I found these lines in the post.  The line that says "headOffset = tool.bodyLength + pivotDistance" seems like it could be the culprit.   What do you think?

[Shannon_IMD]

Yes. That is a very important part of the post. Leave it in. That is how the cam knows how much to offset the tool path. It does show you how the tool length and pivot point interact though. That was my earlier point with the setup.