Tool Path Errors

[richardsalzman]

Hello, I just finished converting a small 2HP benchtop mill to CNC.  My first part on this mill is the Titan 1M (From Titan CNC Acadamy).  Here is the good and bad news:

**Operations:**

1. Facing - Worked perfectly.
2. Adaptive1 - the toolpath that roughs out the contour and pockets - Worked Perfectly.
3. 2D Contour - Fusion created a toolpath the was about 3/8" wider and 3/8" taller than the correct size.  The tool for this toolpath is a 3/8" end mill.  Is there some setting that I may have configured incorrectly to make this happen
4. 2D Pocket1 - This toolpath worked correctly but it left a rough bottom surface (see image).
5. 2D Chamfer (upper section) - Worked great.
6.   2D Chamfer (lower section) - Worked great.
7. Drill Spotting:  No good.  Location of chamfers are in the wrong place.
8.   Deep Drilling:  No good.  Location of holes are in the wrong place.

I have uploaded the fusion file and image of the part.

Any help would be greatly appreciated… Richard

https://www.dropbox.com/s/qyfk8zbj8tyjdki/Titan-1-1M%20PM833%20%28Small%29%20Pre-faced%20Fillet%20v7...

[richardsalzman]

Oops.... Correction.. These are the tool paths that did not work properly (see bold):

**Operations:**

1. Facing - Worked perfectly.
2. Adaptive1 - the toolpath that roughs out the contour and pockets - Worked Perfectly.
3. 2D Contour - Fusion created a toolpath the was about 3/8" wider and 3/8" taller than the correct size.  The tool for this toolpath is a 3/8" end mill.  Is there some setting that I may have configured incorrectly to make this happen
4. 2D Pocket1 - This toolpath worked correctly but it left a rough bottom surface (see image).
5. 2D Chamfer (upper section) - Worked great.
6.   2D Chamfer (lower section) - Worked great.
7. Drill Spotting:  Worked Great.
8.   Deep Drilling:  Worked Great.

[stratosmoulds]

I have toolpath errors also on parallel operation and yestarday was the first time to see these mistakes after working on fusion almost a year now 

[seth.madore]

@stratosmoulds if you could elaborate on what issues you're seeing, please do so. I'm not aware of anything new that's gone wrong, and Parallel is one of the more frequently used toolpaths.

@richardsalzman what do you mean by "3/8" wider and 3/8 taller"? I see that you're using Wear compensation. There should be no value in your tool diameter comp; can you confirm that to be the case?
As for the rough finish; what sort of tooling are you using and are you using coolant? Is this just plain old 6061 sourced from a local vendor? (I ask because there are some real crappy grades of aluminum)

[stratosmoulds]

Hello Seth and thank you for your reply.Here is the issue i am having.

  

[seth.madore]

@stratosmoulds could you share the posted NC code for that toolpath? What post processor are you using? Is it possible to also share the Fusion file? If you don't want to share in publicly, you could email me the link to it (not the file itself): seth dot madore at autodesk dot com

[richardsalzman]

Hello Seth,

I have attached the NC code for the 2D Contour and Fusion files.  Thanks for taking the time to look this over.  What I meant by the toolpath is too big is that the final size of the finished part is 1.9" tall x 3.9" wide.  I am using CNC12 (a Centroid product) that is similar to Mach4 or PathPilot.  When I view the toolpath onscreen, the toolpath is approximately 2.6" tall x 4.7" wide.  This suggests to me that the problem is with the NC code created and not CNC12.  All the other toolpaths ran properly for this part (Except for 2D Contour1).  The image below shows the tool running the toolpath and it is about .185 outbound from the front leading edge of the part.  It is about the same on the left side of the part.   

You noted "There should be no value in your tool diameter comp; can you confirm that to be the case?"  I'm not sure what you meant by this.  I did include the tool diameter in my tool offset library for CNC12.

With respect to the rough bottom surface, I will uploader another image as I can only upload three on this post.  I do believe I am using 6061 aluminum that I purchase from Industrial Metal Supply, but I cannot be sure.  When the Adaptive toolpath was complete, the bottom surfaced looked pretty good.  When I ran the 2D Pocket1 to clean up the bottom surface and sides of the pocket, you can see and feel the lines made by the tool.  See image on next post.

Thanks again for your help.... Richard

[richardsalzman]

Here is the image of the part with blue arrows showing what I was referencing as not a smooth bottom finish.  Laslty, the Post I am using is Centroid Milling Swissi-005.  This is the post that I was directed to use from Centroid.

Thanks... Richard

[richardsalzman]

I forgot to mention.  I am using a solid carbide YG1 3/8" endmill.

[seth.madore]

When using Wear compensation, one does NOT enter any diameter or radius value in their controller, it must be set to zero.

As for the steps in the bottom, are you roughing and finishing with the same tool? (sorry, I don't have your file open right now)

[richardsalzman]

Sorry I am a bit new to this. If I am running a number of toolpaths like this example, am I supposed to remove the diameter value on my tool library when running this the 2D Contour or for all toolpaths? Strange that the other toolpaths worked correctly.

With respect to bottom finish, yes I used the same tool for roughing and finishing.

Richard

[seth.madore]

In your Fusion tool library, you define the tool correctly. At the machine/controller, you do not input any value for diameter, provided you are using Wear compensation. Your Adaptive and Pocket toolpath utilize Computer Compensation, so you could have had a 4" value in the diameter field at the control, and the part would have turned out exactly as you see it.

It looks to me (in regards to the steps) it's possible that it's not liking the .01 chipload, or there is excessive deflection when it runs around the inside perimeter. What happens if you run that same toolpath over again?

[richardsalzman]

Thanks!  I removed the tool diameter from the tool library and the Contour toolpath worked perfectly!  I understand that you are telling Fusion to handle the cutter comp and letting the controller adjust based upon the wear figures only and not the tool diameter.  Thanks so much for your help!!!

I did run 2D Pocket1 again and the surface finish is a little better.  The end mill is brand new and never used before.  As I have no previous milling experience, this surface may be as good as it gets.  You noted "it's possible that it's not liking the .01 chipload".  I do not see where the chipload was set for the 2D Pocket1 toolpath.  Are you suggesting this be changed?

Thanks again... Richard

[seth.madore]

The .01" is based off your Stock to Leave from your Adaptive toolpath. You might want to try an initial 2D Pocket which also uses "Stock To Leave", but set that to .003 axial and radial. Duplicate that toolpath and have the second one leaving no stock. It's my suspicion that you're dealing with machine or tool holder deflection.

[richardsalzman]

Got it.  Thanks for your help.  It is so helpful when you start off at ground zero with no prior experience.  The final step for this part is rigid tapping.  I need to program the parameters for the machine first, then I hope to tap these M4 x .7 holes.  Just curious, the lesson I have been following uses a form tap at 1000 RPM for a large HAAS machine. It was suggested to me that using a standard tap, to tap it at 2000 RPM.  Do you have any thoughts on this or are you aware of a resource to look up speeds & fees for rigid tapping?

Have a great weekend... Richard

[seth.madore]

Always glad to help! Personally, I seldom tap above 5-7 hundred rpm. If you're going to rigid tap that with a cut tap, make sure one of two things is true:

1) Your holes are drilled thru. 

2) If not, then you want a spiral flute (not spiral point) tap, which will pull the chips out of the hole.

3) Does your machine have an encoder on the spindle to allow for rigid tapping? If not, you're going to have to use a floating tap holder which allows for axial movement to take up the mismatch between spindle and Z axis reversal. If your machine doesn't support (and you try) rigid tapping without a floating holder, you will break tap and/or strip out the threads

[seth.madore]

Oh, and make sure you're (preferably) using a cutting oil. Most machine coolants do a decent job of lubrication when tapping, but some...not so much. For a while I was running Blaser Synergy and I could not tap a hole to save my life and had to resort to tapping fluid.  Tap life was poor and frequent acceptance of NO-GO gaging.

[richardsalzman · Accepted solution]

I just stumbled across this video and thought you may be interested:

Better Surface Finishes on Pocket Floors! Testing Different Fusion 360 CAM Toolpaths. - YouTube

Have a nice day... Richard