Tool Holder Creation

[castleworksmotorsports]

Is there a detailed tutorial on creating a tool holder for Fusion 360?

I cannot find my exact tool holder in the libraries and my attempts at creating one have ended poorly with improper Z axis heights and tool breakage.

My exact tool in this case is a BT40 1/2" - 2.5"

On a similar topic I understand why it is important to create a proper tool holder in your library for collision detection, but why can't I simply use any standard one in the library, touch off my tool to the part, enter the tool offset and go....I tried that and ended up breaking bits.

Using other CAM programs, this works fine and I can run, but Fusion is sure making it difficult for me to make the jump to using it full time.

Thanks

Kevin

[Steinwerks]

The tool holder has nothing to do with the tool height definition, and if you are not in need of collision detection then yes, you can just use one of the example holders. The CAT40 holders will be essentially the same in CAM, as they are very similar in reality as well.

How are you breaking tools exactly? The tool should be touched off of your reference as in any machining operation, regardless of software used.

[castleworksmotorsports]

Hi Neal,

OK, I am glad you confirmed that the tool holder does not affect tool height. That is what I would have expected.

I've not had any issues when running my other CAM program (Vectric), all the Z height problems have begun when I made the jump to Fusion.

I created two identical parts in two separate files (attached here), in the first file the G code programmed the tool close to 2.5" above the actual part, and in the second file the z axis came down to the point the tool crashed into the part and broke. In the first, I made an attempt to edit the tool and enter my bit dimensions etc, and in the second I only chose a standard holder and bit from the existing library.

I am clearly doing something wrong within Fusion that is causing my problem, either in my CAM setup or??

I appreciate

[Steinwerks]

The only thing that really stands out here to me in the Setup is the way the stock is defined: Relative with .04" Stock Offsets, making it larger than the nominal size of the part.

Personally I detest this sort of stock mode, and even moreso that it's the default. Personally I would choose Fixed Size Box and input the stock dimensions manually.

I did notice however that you have Tool Orientation on. This is not what Tool Orientation is for, that is for use with a rotary or multi-axis machine to identify the coordinate rotation of an A-, B-, or C-axis or some combination thereof. Turn that off as I suspect that is where your error is coming from, possibly in conjunction with the stock definition.

[castleworksmotorsports]

I see where I had tool orientation turned on in the too high example and turned off in the too low example.

I agree with the stock size, I wish that were not the default.

I'm still really think the problem must be something bigger and not the 0.040" additional stock. The z axis came down, snapped the tool clean off and stopped at a height about 1" above the part and continued on the proper path. The tool I had in the holder was a 5" long 1/2" diameter ball mill. I touched it off to the top f the part, entered the height in the tool offset page as I have always done when I do 2D milling in Vectric.

I mentioned before this is a new post processor, that I have not verified, but it was created from the post I use in Vectric without issue. I think you are the one who previously helped me edit this so the coolant would work. I have attached it here if you wanted to look at it......but my guess is my problem is still within Fusion, as I tried two different tool setup and had two different results.

[Steinwerks]

Yes, I tested your post previously and got what I expected to see. I think this has to do with where your datum is and how you touch off the tool.

Are you using a coordinate definition like G54 on your machine? How do you define the tool offset in the control?

[castleworksmotorsports]

I do use a G54 coordinate definition.

When I touch off a tool, I manually run the tool down to the work piece, read the Z axis value and then enter it into the offset screen attached here.

I agree there must be some datum setting in Fusion that is not correct for my machine or application. I have attached a screen shot that was taken on the first pass of the attached program 1965.tap

I ran some additional tests (taking all tools out so nothing would get broken) to compare the Z axis value on a program from Vectric when it runs to what the Z axis value is when I run a program from Fusion. I saw a big difference.

In the vectric program I ran used tool #3 with the offset value shown in the attached screen shot  of 7.1488..... the first Z movement went down to that value 7.14xx (minus a few thousandths for the first cut)...all was good.

When I ran the Fusion program (see attached G code 1965.tap) it uses tool #6 which has an offset of 7.8638 as shown in the same attached screen shot....the difference was, the first pass Z axis value was what you see on the screen shot 4.9738.....almost 3" lower than it should be. (I took this picture as it ran the first pass on the  part) The G code looks correct in that it is saying to move -0.xx to make it's first pass

I tried this same series of tests using different tool numbers....in each case the Vectric program moved the Z axis to the same position as seen in the offset screen, but the Fusion program moved it to a position that was approximately 3" lower than the value in the offset page.

My thought is this is probably something in Fusion causing the difference, since the post processors are essentially the same post. I have attached the G code from the Vectric program I was using (T Slot Small Precut.tap)

I hope this helps to track down where the difference is. If I can run any additional tests on my end or provide any more data, please let me know.

I really appreciate the help!

Kevin

[Anonymous]

Kevin,

your program 1965.txt calls for T6 M6, but G43 H1. That might be your issue.

David

[castleworksmotorsports]

David,

Any idea where in Fusion it would be getting the G43 H1 command from?

Thanks

Kevin

[Steinwerks]

Well this is where the H value comes from, which seems correct in your example files, and the post is outputting the correct value:

[castleworksmotorsports]

I still keep going back to the fact that it does not move to the tool offset value that is entered on the controller, it moves almost 3" lower. However In an earlier version of the model I changed the tool holder and entered the bit dimensions  it actually moved the tool to a point higher than the tool offset value. It just seems like something in Fusion ignores the tool offset I have entered, and that the tool holder information somehow affects it.

Would it be better to approach this with a fresh look at the post that does work in Vectric on this controller. I've been using it for 6 months, cut a lot of things without issue....and compare it to the post I am using in Fusion to see if something got inadvertently changed?

The Vectric post is "Fanuc0i_ATC.pp" it reads the tool offset correctly and runs fine, with a few small edits I do to the G code (see below) to run it. They are minor but it gets the job done.

The post used in Fusion "Bridgeport_fanuc_coolant_.cps  is a derivative of the vectric post and has been modified by a couple people

For the post "Fanuc0i_ATC.pp" that I use in Vectric, I need to edit the G code in the following manner

1. Remove all line numbers (the controller does not handle 5 digit line number)

2. Remove all M17 and M16 commands (the controller locks up when it encounters these commands)

3. Add in my coolant command M8 and M9 as needed

 I have attached both posts here...NOTE I had to remane the extension on Fanuc0i_ATC.pp to .txt. The forum did not recognize and would not allow .pp files to be attached

I have no experience in editing posts so any help anyone can provide would be greatly appreciated.

Thanks

Kevin

[Steinwerks]

The Vectric post doesn't help, it is not the same as a Fusion or HSM post processor. You say that the Fusion post is a derivative, but this only really  means someone looked at the code that your Vectric post output and modified the Fanuc post to suit that code. Every CAM software has its own post processor configuration and they are never compatible. Some are completely uneditable without specialized software (to keep them proprietary).

I opened your Vectric post in Notepad++ and it is so simple it makes me think that Vectric outputs G-code nearly directly:

+ ================================================
+                                                
+ Fanuc - Vectric machine output configuration file   
+                                                
+ ================================================
+                                                
+ History                                        
+                                                
+ Who    When       What                         
+  ======== ========== ===========================
+ Tony     27/06/2006 Written           
+ Mark     21/10/2008 Amended for 0i, added ATC & new segment    
+ Mark     29/10/2008 Spec amended by customer.      
+ ===============================================

POST_NAME = "Fanuc0i ATC (inch) (*.tap)"

FILE_EXTENSION = "tap"

UNITS = "INCHES"

+ ------------------------------------------------
+    Line terminating characters                 
+ ------------------------------------------------

LINE_ENDING = "[13][10]"

+ ------------------------------------------------
+    Block numbering                             
+ ------------------------------------------------

LINE_NUMBER_START     = 0
LINE_NUMBER_INCREMENT = 10
LINE_NUMBER_MAXIMUM = 999999

+ ================================================
+                                                
+    Formating for variables                     
+                                                
+ ================================================

VAR LINE_NUMBER = [N|A|N|1.0]
VAR SPINDLE_SPEED = [S|A|S|1.0]
VAR FEED_RATE = [F|C|F|1.1]
VAR X_POSITION = [X|C|X|1.4]
VAR Y_POSITION = [Y|C|Y|1.4]
VAR Z_POSITION = [Z|C|Z|1.4]
VAR X_HOME_POSITION = [XH|A|X|1.4]
VAR Y_HOME_POSITION = [YH|A|Y|1.4]
VAR Z_HOME_POSITION = [ZH|A|Z|1.4]

+ ================================================
+                                                
+    Block definitions for toolpath output       
+                                                
+ ================================================

+ ---------------------------------------------------
+  Commands output at the start of the file
+ ---------------------------------------------------

begin HEADER

"%"
"[N] G0 G17 G20 G40 G49 G80 G90 G94"
"[N] T[T] M6"
"[N] G0 X0 Y0"
"[N] [S] M3"
"[N] M17"
"[N] G43 [ZH] H[T]"


+ ---------------------------------------------------
+  Commands output for rapid moves 
+ ---------------------------------------------------

begin RAPID_MOVE

"[N] G0 [X] [Y] [Z]"


+ ---------------------------------------------------
+  Commands output for the first feed rate move
+ ---------------------------------------------------

begin FIRST_FEED_MOVE

"[N] G1 [X] [Y] [Z] [F]"


+ ---------------------------------------------------
+  Commands output for feed rate moves
+ ---------------------------------------------------

begin FEED_MOVE

"[N] [X] [Y] [Z]"

+ ---------------------------------------------------
+  Commands output at toolchange
+ ---------------------------------------------------

begin TOOLCHANGE

"[N] M5"
"[N] G0 G91 G30 Z0 M16"
"[N] G90"
"[N] T[T] M6"
"[N] G0 X0 Y0"
"[N] [S] M3"
"[N] G43 [ZH] H[T] M17"

+ ---------------------------------------------------
+  Commands output at New Segment
+ ---------------------------------------------------

+ begin NEW_SEGMENT

+ "[N] G0 [ZH]"
+ "[N] M5"
+ "[N] [S] M3"

+ ---------------------------------------------------
+  Commands output at the end of the file
+ ---------------------------------------------------

begin FOOTER

"[N] [ZH]"
"[N] M5"
"[N] G0 X0 Y0"
"[N] G91 G30 Z0 M16"
"[N] M30"
%

It would likely be very simple to edit out the issues you see in this post though.

There's still nothing in the code that would be different here, except for G30.

Is G30 a secondary home position?

[castleworksmotorsports]

Hi Neal,

Honestly I do not know what G30 is, I'm just not that well versed in G code. Could that be causing the problem of the tool height?

I have only used G54 when setting my origin and go from there.

[Steinwerks]

1) What exact control does your machine have?

2) There is no G54 callout in either of the programs you shared, so unless the control defaults to using G54, I don't even know that it's using a work coordinate offset.

[Anonymous]

If you post a new program, does it really give you H01 again? That should be almost impossible. Is the .txt file manually edited?

David

[castleworksmotorsports]

Hi Neal,

Thanks for your patience and help on this. I really do want to get to the point where I can use Fusion as my only CAD CAM product.

The controller is a GE Fanuc Series O-Mate M  (see attached image of the controller)

I am really new to using this type of CNC, so let me walk you through my process when I first load material into the vise and how I go about setting the origin. I created these instructions with the help of the previous owner of the machine. These are the steps I follow each time. I realize they are over simplified, but I wrote them so anyone helping me in the shop could follow them.

I have also included screen shots of the Work Coordinates page, the tool offset page and Operator Alarm Page
 

After loading your work piece into the machine you need to tell the CNC where 0,0 (X,Y) is located. Perform the following procedure.

   1 Load the Edgefinder tool using the tool loading procedure above.
   2 Press the OPR ALARM button and use the arrow keys to highlight MDI.
   3 Press the PRGRM button.
   4 Type in M3 and press the INPUT button (this specifies CW rotation of the spindle)
   5 Type in S800 and press the INPUT button (Sxxx specifies the RPM for the spindle)
   6 Type G59 and press the INPUT button.
   7 Press the green CYCLE START button (arrows in a square pattern with a 1 in the middle).


NOTE, now the X,Y coordinates will be measured from the Machine Home 0,0,0 and they should all be negative.

   8  Press the OPR ALARM button and highlight HNDL using the arrow keys.
   9 Move the table and spindle so the edge finder is at the location you want to be your reference point.
   10 Write down the values for X and Y including the negative sign.
   11 The edge finder is 0.2” in diameter so you need to add or subtract 0.1” from the readings to make sure you are specifying the center of the tool is on the reference point. These are your new values for X,Y
   12 Press the MENU OFFSET button.
   13 Press the MENU OFFSET button until you come to the WORK COORDINATES page.
   14 Using the arrow keys, cursor to 01.
   15 Type in X-_ _ _ using the value from step 11.
   16 Press INPUT.
   17 Type in Y-_ _ _ using the value from step 11.
   18 Press INPUT.
   19 Press the OPR ALARM button and use the arrow keys to highlight MDI.
   20 Press the PRGM button.
   21 Type G54 and press the INPUT button.
   22 Press the CYCLE START button.

Note now the X,Y locations will be measured from the reference point in the Work Coordinates page and can be positive or negative.

 SETTING TOOL OFFSET:

NOTE: I am setting up the offsets so the offset number corresponds to the tool number in the carousel.

   1 Load the actual tool you will be using (See section 2.0 for these instructions)
   2 Press the OPR ALARM button and highlight HNDL using the arrow keys.
   3 Move the spindle down to the top of the part until it just touches the top surface of the part.
   4 Write down the Z position
   5 Go to the offset page by pressing MENU OFFSET.

     Arrow down to the tool you are setting the offset on.
  6  Type in the value from step 4 and press INPUT.

7 Repeat the process for each tool you will be using for this particular part.

[castleworksmotorsports]

Adding an overall image of my controller

[castleworksmotorsports]

David,

The file 1965.txt is direct from Fusion completely unedited (I only changed the extension to txt so I could post it here)

Do you mean post the same model again, or a different model altogether? I'm happy to try anything if it will help track down the problem.

[Anonymous]

Just post the same model. 😀

[castleworksmotorsports]

David,

Here is the new post, only the file extension was changed from .tap to .txt in order to post on the forum.

Thanks

Kevin