Which 5 axis toolpath is best for this, any tips are greatly appreciated and if I can produce a good toolpath, ill get u some brews

[SIMPLEEDABESST]

So the finish has to be spot on because its forming nitinol wire for stents

Im using Mastercam 2023

toolpath.pdf

[#Rekd™]

Without a Mastercam file it is just a guessing game. Flow 5 Axis? Unified?

 

[SIMPLEEDABESST]

Here u go

T-7866-1.STEP

Thank u

[SIMPLEEDABESST]

i just need the groove finish toolpath using .035 ball mill

[#Rekd™]

That is a CAD file, post a VALID Mastercam Ziptogo file. This will allow people to see what machine (type of machine and configuration). 

 

[SIMPLEEDABESST]

Ok sorry , any help is really appreciated, i've spent a week trying alot of toolpaths, I have 4 sets of these which once I have a good ruff/fin toolpaths I just export the path, and life is wonderful again. Just the groove, everything else is done. 5 axis machine but 3 axis path is fine

T-7866-1.MCAM-CONTENT

[Brad St.]

When your stating the best that still doesn't give us the details you need for the finish. 

Are you simply looking for a controlled scallop height or do you want the scallops to be in the same flow pattern as the wire groove?

I've done these in the past with 3 axis machines. Are you looking to use 5 axis simply for getting the tool off the tip for better finish and due to tool size needed?

Not trying to be picky or anal, just looking to give you the right feedback to help you get the best finish you need

[SIMPLEEDABESST]

Yes and thank u. The width and Height for the groove are different for every set, only one remains the same. The width and Height are +/- .002 inches and the bottom radius max .018. I can select geometry and avoidance just fine, I usually use flowline with a .001 stepover which they dont call out a particular finish but any lines in the groove get transferred onto the Stent and if you've done medical parts thats unacceptable,. These go into a salt pot later to form Memery metal

[SIMPLEEDABESST]

Im on the 5 axis because it was free not that it's necessary. If you can do simultaneous 5 axis that would be fine as long as I can export the path and use it again and again

[#Rekd™]

Got a decent looking toolpath with Unified controlling the tool Axis "From Chain". Still needs some refining but it looks decent.

 

 

[rgrin]

I personally would break it up into a couple toolpaths, but if you want just one, unified auto parallel works well.  I just did surface with tilt and put a cone limit set at 8 degrees.  Got an alright toolpath

[SIMPLEEDABESST]

That looks great let me try it , Ill cash app you some money for beer, give me until afternoon

[SIMPLEEDABESST]

How do I avoid all the rapid moves up and down?

Thats usually not a problem but it just takes one to either break the tool or gouge the part

[rgrin]

I make no guarantees. I did not collision check this at all.

I made this in MCAM2022.  It looked better in 2024. I think they updated the algorithm for auto parallel in 2024?

I switched from one way cutting to spiral and that got rid of alot of the rapid moves.

Play with it and see what you can get

T-7866-1-2022.mcam

[SIMPLEEDABESST]

So I like it, one issue is my position, which im figuring that out out. WCS, Tool planes.

Another is c axis is spinning around and around until the angle is thousands of degrees from where it started, can that be fixed

I actually have it standing up like this, on a haastoolpath.pdf

[rgrin]

If you set the program planes to how you have it modelled, it shouldn't do any full rotations.  It will adjust the angle of the B/C simultaneously.  

Should more or less be able to just create a new work plane based off your actual "Top" Plane but then orient the Z Axis to be pointing at the flat surface.  Then use the "Top" as WCS and the new plane as your T-plane.  T-plane is what sets your tool orientation.

I would imagine that any modernish Haas 5-axis would have infinite C-axis anyways. So, even if you ran it how I have it oriented, you should be just fine.

[SIMPLEEDABESST]

Good god this F'in job is frustrating, now it completely changes the position the endmill starts simply with changing from unified guide parallel to automatic parallel for no reason. didn't move the model but it changes the g code positioning 3/4" on x

yeah its a haas issue we determined that

[SIMPLEEDABESST]

OK I wanna thank u and buy u some coffee or beer so pm WITH YOUR CASHAPP HANDLE

[rgrin]

12 hours ago, SIMPLEEDABESST said:

OK I wanna thank u and buy u some coffee or beer so pm WITH YOUR CASHAPP HANDLE

Lol, all good dude! I don't have cashapp.  We are all happy to help here and I like to use these as little mini exercises for myself to stay fresh.  Not often that I actually get to program full 5 axis

[Brad St.]

Here's one way I would  tend to flavored it for a finish pass.

T-7866-1-2022_6-26-2024.MCAM-CONTENT

[rgrin]

One thing I wanted to mention is that you do not need to use 3D or multi axis toolpaths.  Often times, you can get easier and better results with 2D.  In this example, the code will be able to do all arcs and lines and give incredibly clean motion with a fraction of the code necessary.

 

 

T-7866-1-2022-2D Sweep.mcam

[SIMPLEEDABESST]

Rgrin’s original toolpath is nice left a good finish but is cutting as if it’s on center ball mill mode and over cutting can’t figure out why

Only on the sides though

[SIMPLEEDABESST]

Brad ST - Nothing came with yours - it said I needed Migration and to choose files, Im on 2023 so It should work just fine.

And Rgrin, 2D looks nice I would still need the rest of it thought . Your original AUto parallel is what ill go with just need to figure out why its not offsetting properly

[#Rekd™]

3 hours ago, SIMPLEEDABESST said:

need to figure out why its not offsetting properly

A sub menu under Cut Parameters, set to contact mode 

[Brad St.]

Sorry my apologies, yes I'm on 2024.