Thread Milling Rapid Collision with stock error

[winteragera]

Hi all, before I continue, I just want to say I am very new to CNC and Fusion360 CAM

My goal is to make a "water distribution plate" that accepts G1/4 BSP threading with M4 screws holding two-piece of cast acrylic sheet together.

I am trying to thread mill some M4 screw holes into 12.7mm cast acrylic sheet. However, I'm running into one major problem at the moment. When I try to simulate the threading process, I keep getting these red bads and it indicates "Rapid collision with stock" 

Some of the things I've tried:

-Checking my tool size is correct

-Setting the top height to "Stock top: 0mm" in the height tab

-Making sure the design hole depth is NOT longer than flute length of the thread mill cutter

I am using a thread mill cutter from Datron and they haven't provided me the tool measurement so I gave it a shot myself. Please check if anything is wrong.

[seth.madore]

At this point in time, selecting a single operation and Simulating it will not give you the result of everything that theoretically should have occurred before. To avoid getting false alarms, simulate everything you got

[Anonymous]

Something to check would be your lead in (lead out) values on your linking page.

That's the last tab on the right in threading. Lets say your major diameter M4 thread is

.158 t0 .161 . This means your minor is, lets say .136 diameter. If your tool is 3mm (.1181)

your lead in/out has to be small enough to allow clearance. Hope this helps!   

[winteragera]

When I try to simulate everything, it still gives me the error 😞

[Richard.stubley]

Hi @winteragera,

Could you attach your Fusion project please

File> Export > export as .f3d

[winteragera]

I just tried your method. Unfortunately, changing the horizontal and vertical lead in/out in the linking tabdoesn't help. There's still the error or "Rapid Collision with stock"

[winteragera]

Yep, hope this gets solve soon. 

[seth.madore]

You did not have any drilling cycle before the threadmilling. As such, it considered that the holes were still solid. Adding a drill cycle and then simulating both toolpaths yields no collisions:

 

[winteragera]

Keep in mind I have a thread mill cutter. So it plunges into the materials and does the threadings at the same time. 

EDIT:

With the drill (full retract) operations before the thread operation, it still gives me an error. Even with simulating everything and not simulating the threading itself 

EDIT 2: My issue now is the deep drilling operation doesn't cover the whole diameter of the hole. How do I fix that? 

[seth.madore]

Okay then. The threading toolpath isn't going to be your "one and done" solution, as there is nothing baked into these toolpaths to generate both a drill cycle AND a threading cycle. You will need to program one hole with a Drill followed by a Threading cycle and then put that into a Pattern.

As for the alarm, I'm not seeing that on my end....

[DarthBane55]

The tool does not need a hole, but I doubt that Fusion can handle that type of threadmill directly.  I think you will always get the collision, because the threadmills inside Fusion are not made to cut from the bottom (I think).  You also cannot plunge with the tool, you need to helix with the proper pitch and diameter.   You might actually have to use the "bore" cycle and adjust the pitch.  Maybe the threadmill operation would work, but you need to start from the very top.

Video showing similar tool in action: https://www.youtube.com/watch?time_continue=4&v=iUl42whFisI&feature=emb_logo

For your drill question, it seems to me that you got the wrong drill is all...  but you don't need a drill for this tool.

[kamil.malec94]

If you add drilling cycle before your Threading cycle and simulate both, you do not get any errors. I always do "Lead to Center" in the Linking Tab, this way I know I will not hit the stock.  

[rhdfmail]

Threadmilling (2D-thread) works fine from bottom to top. You just select climb-milling 

With combined drills/threadmills it might be possible to trick the operation to drill and then mill
setting the heights so it starts lead in from top, lead feed = feed for drilling, lead to/from center
To make it feed from top, set the safe distance under linking to the same value as your thread/hole depth

Not tested more than a quick test in fusion looking at the toolpaths that is generated

[seth.madore]

One question to @winteragera is the tool intended to:

A) Drill the hole and then thread mill it

B) Conventional mill into the part, creating the hole and the thread in the same motion

[DarthBane55]

---

@rhdfmail wrote:

Threadmilling (2D-thread) works fine from bottom to top. You just select climb-milling 

With combined drills/threadmills it might be possible to trick the operation to drill and then mill
setting the heights so it starts lead in from top, lead feed = feed for drilling, lead to/from center
To make it feed from top, set the safe distance under linking to the same value as your thread/hole depth

Not tested more than a quick test in fusion looking at the toolpaths that is generated

---

He needs to start from the top, if you saw the tool, it mills the hole, no drill required.  But your comment about the climb milling starting from bottom, which was my concern for his tool,  and why I suggested to use "bore" operation, I think that choosing conventional mill will force it to start from the top, which is what OP needs to do with this particular tool.  I wasn't sure we could force it to start from the top, but your comment made me realize that the conventional mill will do this.

[seth.madore]

Yep!

[winteragera]

This might be a possible solution. I now need to wait for Datron to reply with how I should input this Thread mill cutter bit information into Fusion first. Apparently Fusion doesn't like the tool to be classified as "Thread Mill"

They also haven't updated their tool library. 

[seth.madore]

As I mentioned above, does the tool require that you first have a bore operation and then a thread operation, or does it do it all in one shot?

[winteragera]

So it seems like there is no way to get around this. I got replied back from Datron after 2 days (that's why I haven't updated this topic) and they have the exact same problem. The tool itself plunges into the material and does the threading AT THE SAME TIME.

Keep in mind they used the thread operation and they still got the "Rapid Collision with Stock" error message. 

[DarthBane55 · Accepted solution]

It doesn't plunge, it helixes down.  I would just create an endmill with appropriate diameter, and understand the that actual thread would not be shown in the simulation.  Then you won't have the collision alarm.  In this case tho, you do need to use "bore" cycle and adjust the pitch correctly, and make sure the helix is going down in the right direction.  Or the other way, is to use a threadmill tool and operation, but ignore the collision (probably better with this).