Threadmill Z height milling depth consistently short

[Ryan_Mahadocon]

Whenever i threadmill internal or external threads, it appears that something isnt defined correctly to get the z height im targeting. for instance, heres what my sim shows vs what im actually cutting. I consistently plunge too shallow.

 

I keep thinking its something in the way i defined that threadmill in the tool library, but i cant figure out what it is.  

The only hint i see anywhere that i dont have something correctly defined is the scaling the picture in my library shows. the total width of the flute is .065", but the picture scaling seems to represent the flute as only about ~.035".

Any suggestions would be appreciated

[programming2C78B]

Your z depth is the bottom of the tool, not the bottom of the thread. I also am unsure if your thread pitch info is correct when there is only a single tooth.

[Ryan_Mahadocon]

Thanks for the feedback, I understand the tool height and my toolpath height selection is what determines the cut depth. However, that is only the case when the axial end of the tool is a cutting face. I set my z height of this threadmill the same way ive set the z height for all of my other tools (which cut the appropriate z heights). the issue is that fusion seems to think the 60deg flute is offset from the bottom of the tool, less than it actually is (see the last picture in my first post as a refrence). 

Think of it as if the threadmill flute was like an inch up the neck, fusion would know that geometry to accurately hit the z height your actually cutting. 

Still hoping someone on here has faced this before. I couldnt find anything searching the forum. 

Thanks!

[seth.madore]

Would you be able to share your Fusion file here?
File > Export > Save to local folder, return to thread and attach the .f3d/.f3z file in your reply.

[Ryan_Mahadocon]

Hi Seth,

Thanks for reaching out. Happy to share the file. The threading opp im talking about is Opp2. Have any preliminary thoughts on what might be happening here? Thanks!

[seth.madore]

Both of your Setups raise more questions than answers 😂

What's the deal with your Stock and where you have your WCS set?

In regards to the threading toolpath; it appears to be correct. Yes, the image that's reflected of your tool doesn't look right, but it's purely a cosmetic thing and not going to produce incorrect code. The g-code Z heights are based on the tip of the tool. So, if you're getting different results at the machine, I would look there first to confirm your WCS and your tool height is set correctly.

What is your machine and control? Toolchanger, or setting each tool individually?

[Ryan_Mahadocon]

Hi Seth,

I really appreciate the feedback. Im still working to understand how Fusion nests fixturing , manufacturing models, and the whole design space, so i apologize for the apparent experimentation. Sometimes i want to run the first two Opp's in my vise, and the remaining opps in a fixture, so trying to get a grasp on that.

A bit about that WCS. My machine is a Tree Journeyman 310, with a Delta 20 Control. This control only has one WCS at a time, and so when i power up the machine, i indicate in on the back left corner on my hard jaws, and set the Z height to the top of my parallels, allowing me to run all of my opps off a common WCS. This saves me a ton of time from the standpoint, that indicating in requires touching off using a reference tool, as well as a edge finder. Setting up this way saves me about 5 minutes per WCS indication if i can use a common WCS between all of my opps.

Thanks for the info about the Cosmetic representation. To set tools on on the J310, i have a reference tool, that the control uses as its "0" height.  Using a Tool height indicator, i touch the pad using the reference tool, zero the Z portion of my WCS, change tools, and touch off the pad to that same height. I then use my 'tool cal' function on the machine that automatically calculates the difference in height between my z reference height. This gets saved in my machines tool library, which is referenced every time the tool is called.

Ill reset the tool height for the threadmill, and re-run the part to see if the outcome changes, ill report back what i find. Thanks!

-Ryan

[Ryan_Mahadocon]

Seth, 

Can you by chance offer an explanation for how fusion knows where the cutting point of that flute is on that shank? Fusions defining tool geometry doesnt ask for Flute height (radial length of the flute), or neck diameter, so even given the angle of the cutter, the height of that flute doesnt seem to be able to be defined. 

[leo.castellon · Accepted solution]

As Seth pointed out, "The g-code Z heights are based on the tip of the tool." It doesn't account for the actual cutting edge of the thread mill. This is to prevent for an example, the thread mill going too deep in a blind hole. If the thread mill went into the blind hole where the actual cutting tip is, then you would break the tool. In this particular case, you would add a thread relief so that the item would screw in all the way. In your case, just add some extra Z cutting depth so that the thread mill cuts a complete thread.

LeoC

[Ryan_Mahadocon]

Thanks Leo,

This is where my thoughts were headed. The solution you offered will work in most cases i think.  its interesting to find out in my example that i cant get an accurate simulation. I think threading a blind hole, and needing all the threads you can get, is probably not a common thing many people come up against. I was relying on the simulation to give be a 'warm and fuzzy' feeling about how many threads i was going to be engaging. i have an idea on how to fix it in my case (im going to source much smaller thread mill i can to get as much Z depth in that blind hole) but as you pointed out, in my case, my limiting factor for what was actually being produced is probably constrained by the z height of my tool, and the depth of the thread was being mis-represented in the simulation.