Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Pocket depth setting and tool length changing?

jgaertner
Collaborator

Pocket depth setting and tool length changing?

jgaertner
Collaborator
Collaborator

Hello Forum,

 

I am new to Fusion360 and working with a new Tormach 1100PCNC. Double whammy. I have done CNC before.

 

I am trying to practice using 360 by cutting a 2.5" Diameter closed pocket .5" deep in a piece of 3/4" MDF with a 1/4" diameter HSS end mill that has .623 long flutes. I have created the pocket in my drawing and assigned a cutting tool (1/4" end mill with my set parameters) but what I am not sure about (and have not found it in the tutorials) is how the CAM knows what depth to cut the pocket (feature)? I know about the Heights tab but it is unclear as to whether I have to set the depth of the pocket or doesd Fushion know how deep to cut the pocket because I selected the bottom of the pocket?

 

So when I run the program, the mill goes deeper than I want it to in the sample material. I have Z referenced my tool according to the PCNC manual. Any thoughts or suggestions so I can narrow my problem down to ether CAM error or CNC mill set up error (all are my doing).

 

Thanks.

0 Likes
Reply
2,541 Views
17 Replies
Replies (17)

Steinwerks
Mentor
Mentor
Not sure without seeing the part file, but I suspect one thing first and foremost: your stock definition.

How much deeper is your pocket than the model? The code should output to the geometry if you selected the contour (or face) at the bottom, but if your stock is defined as .04" oversize (the default) then if you touch off the top of stock that is meant to be Z0, you'll get deeper features by virtue of the stock definition.

That's my first guess anyway.
Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

jgaertner
Collaborator
Collaborator

Steinwrks,  

 

Thanks for your reply!

 

I will have to check. The material is specified at 3/4" thick. I did not change in Fushion360 the stock definition!

 

But that may be the issue. I do not know how to post the original file cause its still not clear to me, where it is being saved? on my computer or in the "cloud" with Fushion 360? I wish this was more straighth forward like the software I am use to.

 

I will work on this and get back to the thread with what I find.

 

Jgaertner

0 Likes

Steinwerks
Mentor
Mentor
It's in the cloud.

If you go to "File -> Export" you can choose the .F3D file type and attach it here though.

What was your previous CAM software?
Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

jgaertner
Collaborator
Collaborator

My previous experience is with a CNC router we had using BobCAM which I felt was not a very good program. We sold the machine because we just found it was not productive $$$ wise for our shop. I have been using AutoCAD since 1990's and SolidWorks since 2010. We use SW 2014 most of the time but I am giving Fusion a try since we bought this new CNC mill.

 

jgaertner

0 Likes

jgaertner
Collaborator
Collaborator

Hello Forum,

 

I think I have discovered why my Tormach Mill was machining deeper than I wanted. I spoke to the people at Tormach after running the G code for a second time removing any top height (I did not need to face the piece of MDF I was practicing on) and the G code still ran my mill 0.362" deeper than I wanted. The problem is with the G code being generated by Fusion. It is not changing the H (tool Height) to match the tool library tool I selected. So the G code thought I was using tool #1 in my tool library when in actuality I was using tool #2.

 

Maybe this is in the Post Processor file or may be, since I am new at Fusion, I missed something? But once I manually changed the H# to match the tool I was using, the program ran fine.

 

Hope this helps others....

 

Jgaertner

0 Likes

kb9ydn
Advisor
Advisor

@jgaertner wrote:

Hello Forum,

 

I think I have discovered why my Tormach Mill was machining deeper than I wanted. I spoke to the people at Tormach after running the G code for a second time removing any top height (I did not need to face the piece of MDF I was practicing on) and the G code still ran my mill 0.362" deeper than I wanted. The problem is with the G code being generated by Fusion. It is not changing the H (tool Height) to match the tool library tool I selected. So the G code thought I was using tool #1 in my tool library when in actuality I was using tool #2.

 

Maybe this is in the Post Processor file or may be, since I am new at Fusion, I missed something? But once I manually changed the H# to match the tool I was using, the program ran fine.

 

Hope this helps others....

 

Jgaertner


 

 

Yeah, I'm pretty sure this is because the tool library lets you have different numbers for the tool number and length/diameter offsets.  This is supposedly intentional but it seems like a very bad idea to me.

 

 

ToolNumbers.PNG

 

 

C|

0 Likes

Steinwerks
Mentor
Mentor
Sorry I didn't get back earlier.

This is intentional because many times it is useful to use the same tool with different offsets for different features that may have varying tolerances. Also it can be useful for developing tool libraries for machines that have multiple tool offsets but limited pockets. For example in our Fadal we have (I think) 99 tool offsets, but only 21 pockets in our ATC, and every ATC pocket is linked to the T number. If I had enough tooling and didn't want to touch off all the time, I would have multiple tools set up as, say, T1, but could use, say, 31 for the Length and Diameter offsets to keep the tool stored.

If you hit Tab on the keyboard when you change the Number is should auto-update the offsets, so be careful when just hitting the OK button when the Number field is the active field.
Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
1 Like

kb9ydn
Advisor
Advisor

@Steinwerks wrote:
Sorry I didn't get back earlier.

This is intentional because many times it is useful to use the same tool with different offsets for different features that may have varying tolerances. Also it can be useful for developing tool libraries for machines that have multiple tool offsets but limited pockets. For example in our Fadal we have (I think) 99 tool offsets, but only 21 pockets in our ATC, and every ATC pocket is linked to the T number. If I had enough tooling and didn't want to touch off all the time, I would have multiple tools set up as, say, T1, but could use, say, 31 for the Length and Diameter offsets to keep the tool stored.

If you hit Tab on the keyboard when you change the Number is should auto-update the offsets, so be careful when just hitting the OK button when the Number field is the active field.

 

 

Hitting the tab key does not update the offsets, it only moves the focus to the next box.  You still have to type in the value or use the increment/decrement buttons.

 

I would prefer if there was a way to link these values together, like the old tool library used to do.

 

 

C|

0 Likes

Stuart-H
Collaborator
Collaborator

Yep that has caught me out a few times now I am very careful when setting up f360 tool table and as a second sanity check I use MSM on top of mach3 so I make sure that tool table is in step

 

 

Mac Studio M1Max and MacBook Pro M1
0 Likes

Steinwerks
Mentor
Mentor
You're right, tabbing doesn't do it. But mine updates automatically when I change the first field.
Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

kb9ydn
Advisor
Advisor

@Steinwerks wrote:
You're right, tabbing doesn't do it. But mine updates automatically when I change the first field.

 

 

???  So you're saying when you change the tool number, the length and diameter offsets also change automatically to match the tool number?  Mine doesn't do that and I really wish it did.

That's the way it used to work with the old tool library.  HSMWorks and HSMXpress (for Solidworks) still work this way but Fusion (and I'm pretty sure Inventor HSM) don't.  At least my Fusion doesn't.

 

 

C|

0 Likes

Steinwerks
Mentor
Mentor
Yes, mine updates automatically, at least when creating a new tool. I tried selecting other fields, tabbing through and returning to the tool number field, always updated the offset fields. I can make a screencast later. What's disturbing is that this apparently isn't consistent between installs.
Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

kb9ydn
Advisor
Advisor

@Steinwerks wrote:
Yes, mine updates automatically, at least when creating a new tool. I tried selecting other fields, tabbing through and returning to the tool number field, always updated the offset fields. I can make a screencast later. What's disturbing is that this apparently isn't consistent between installs.

 

 

Oh, I'm not creating a new tool, I'm editing an existing tool.  When creating a new tool the fields are updated automatically.

 

 

C|

0 Likes

Steinwerks
Mentor
Mentor
Ah yes, same experience here. Not a good default behavior, I agree.
Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

jeff.walters
Advisor
Advisor

I have submitted an enhancement request (CAM-4115) for a check box to link the length and diameter offset to the tool number. This should give the flexibility to run either way.

 

link offsets.png

Jeff Walters
Senior Support Engineer, CAM
2 Likes

kb9ydn
Advisor
Advisor

@jeff.walters wrote:

I have submitted an enhancement request (CAM-4115) for a check box to link the length and diameter offset to the tool number. This should give the flexibility to run either way.

 

link offsets.png


 

 

That would be great!  Thanks Jeff!

 

 

C|

0 Likes

Stuart-H
Collaborator
Collaborator

thanks Jeff you get a star for that 

 

 

Stuart

Mac Studio M1Max and MacBook Pro M1
0 Likes