parker hannifin

[magpiemachining]

Need some help programming a parker hannifin slot. anyone have experience doing this with fusion? I can not get the lead in and out correct. that may be due to the tool i set up. it is similar to a dovetail. only issue is  i never used the neck diameter as the cutter radius which is how i am seeing fusion wants the tool set.  also a tech told me that is how it is calculated. He also could not get the lead in and out correct and said there is no process for this type of slot and would get back to me.  anyone familiar with this knows there is no room. cuts are to be taken radially and there is no drop hole in this design. fusion wants to retract with the cutter under the slot. no good. fusion also wants to come out of the slot and enter at a different location to make another pass.  i placed a point in the center to indicate an "entry point" but can get it to exit there and retract. Any help? thank you for reading

[LibertyMachine]

I've had to cut a few of them. I find that by playing with the lead-in/out settings I can achieve mostly what I'm looking for.

Can you export and share the model, or an example of what you are encountering?

[magpiemachining]

Hi. thyank you for thye reply. i believe this is all due to the way the tool geometry is calculated. using the neck diameter doesnt seem right unless the flute diameter is the same or if i was needeing to  use the the larger radius on  an angle mill. you can see in the tool library i added the tool with the dovetail and modified the corners. this doesnt work because the diameter it wants is at the neck. you can see this also how the cutter violates the line in the 2d drawing.i drew the tool on a seperate sketch in that same file. the other file is a model i was working on previously. im sure there is a lot wrong there because i was changing so much trying different things.

[LibertyMachine]

Are you using a Harvey O-Ring cutter?

[magpiemachining]

yes

[magpiemachining]

i used a dovetail from the library and tried to modify the corners with a radius. 

[LibertyMachine]

Yep, I see the issue. Gimme a bit to get my job up and running and I'll bounce back to your issue.

[LibertyMachine]

Sincere apologies in the delay in response.

Gotta say; I think they stuffed it up bad on dovetail cutters. It's definition is questionable at best, and I'm not entirely certain it's from the neck diameter. 

Oh, the tool is defined by the neck diameter, which makes zero sense, but I don't believe the toolpath is actually driven by the neck diameter. If that makes any sense....

At any rate, here is your part back. I made a duplicate body so I could split it in half and observe the toolpath parallel to it's travel. 

I created a new tool replicating as close as I could to what Harvey calls out. I've also done a sketch of the tool as Harvey says it should be and I feel it's pretty darn close to what you need.

My method of tweaking it in was simply adding "Stock to Leave" until I was satisfied with the results.

@jeff.pek @al.whatmough, could you lend some insight into why and how to define a Dovetail cutter? I searched on the HSM board and the most common answer was "Define a Form Cutter".

Am I correct in seeing that it's driven or defined by "Neck Diameter"? If so, may I ask "Why?" It's not a controlled feature of the tool, unlike the theoretical sharp point or the physical overall diameter

[randyT9V9C]

Does Fusion 360 support ramp along path? The issue appears to be due to cutter comp and the required dog leg start. This would be a lot easier if he could use a hole start cutter. 😉

 Ok, I see your reworked cutter and paths. 

[LibertyMachine]

Yes, Fusion does support Ramp along path. 

The toolpath that I laid out does a fine job of plunging in on center, picking up Comp, making a race around, and repeat the process for the other side of the wall. You can easily duplicate the operation, leave some stock (also need to reduce your lead-in/out) and you would be good to go.

The bigger problem I think he was running into is the poor method of tool definition. Would really like to hear some thoughts from the big guys why it is how it is

[randyT9V9C]

Yeah, your reworked tool worked much better. 🙂

[LibertyMachine]

I'd be lying if I said it was easy enough to calculate out how to define the tool and where it's being driven from. I tried splitting the faces at various height intervals to drive the tool and nothing seemed to be able to produce a solid cut WITHOUT fiddling with "Stock to Leave". This should be something that can be calculated rather simple, but it's not. Perhaps I am ignorant of the math required..

[magpiemachining]

I made the partpart befor.I wiggled through it. changed this and that. i just got a mold to build with this geometry in 4 plates.and a sprue puller which uses the same geometry. actaully smaller. but i thought this was a good time to reach out to the forums and see if anyone else had this issue this type of geometry and tooling. Thanx for for your help. Im glad someone else was able to see the tool problem. please follow up with any info from the engineering guys. Thanx again

[fonsecr]

Hi @LibertyMachine,

The dovetail definition is not desired as it is now. The corner radius is added to the diameter instead at the moment - easiest to see if you set the taper angle to 0deg. Which is opposite to the bullnose tool type. We need to make sure we match the tool definition in the vendor tool catalogs. We just havn't got around to this task yet.

I'll ask team to review it.

[LibertyMachine]

Ok, I see that now. That makes more sense than how I first thought it was defined. 

However, I'm still not certain on how to perform geometry selection without constant fiddling with the "Stock to Leave command".

If I model a dovetail feature with no fillet and then define a dovetail mill with no radius, I am able to select the root of the dovetail and create a tool path with ease. No fiddling with the Stock to Leave.

However, if I correctly define a dovetail cutter with a radius on it, I now need to start guessing what value I should place in the "stock to leave". Turns out I needed to have a .024" radial value on this tool (.375" dovetail with .010 radii, defined as a .355 diameter):

And in the case of dealing with models that have the fillets built into them, in the case of the Parker Hannafin O-rings, what feature on the model are you supposed to select? I tried splitting the faces at several different layers to see what I could generate with little guesswork, and everywhere I selected seemed to require a "Stock to Leave".  I tried both the tangent point where the radius meets the floor, as well as the tangent point where the radius meets the angle. Both required fiddling of "Stock to leave". Should we model the parts with no fillets? But even then, it still requires some value in "Stock to Leave".

Is there an expression that can be made to make this less painful? Am I missing something silly that would make all this a non-issue?

[magpiemachining]

i have been fiddling with this. . this is a new slot for a mold. smaller and a simple circle. i drew a 2d sketch rather than model the groove as it makes no difference for this test. the tool  required is a .113 diameter tool harvey oring tool. I tried the approach of using a flat end mill  with the radius of the oring tool and simlply used the cutter comp to get to the contour edge. same process as if you were to use a tapered end mill. you would walk the smallest or largest diameter to the contour without defining the taper of the end mill. sort of tricking the control. it doesnt know its a tapered end mill.  on the lead in move the cutter still will not plunge at the point i pick no matter what lead i put in. its close and can be adjusted in the post. the lead out is the distance or the cutter radius and the contour. now the other issue arises. when i tweeked in the first contour to where i wanted it and worked, i duplicated the path and reselected the geometry to do the other side. i selecteed the same way in the same location aas the first. you can see it created 2 different paths. the second seems more desireable as it sort of ramps in and starts over the point selected. the first one starts in left field and ends in right field.why would it produce 2 different paths from duplicating the path? and why wont it plunge at the point selected?

[cj.abraham]

Ticket CAM-8217

[LibertyMachine]

@cj.abraham, could you expand on this? What issue is CAM-8217 logged for?

[cj.abraham]

Changing the definition to define the diameter as the total width, including the corner radii. Like Major diameter as it is shown in this image:

[LibertyMachine]

Excellent!

Any insight into my query up above, regarding proper geometry selection in modeled o-ring grooves?