5 axis curve?

[JMahon]

Hello all,

I am trying to do a 5 axis curve to run the corner of an endmill along the channels to cut these rasps, but am having trouble getting my tool to do what I want it to. I am still new to multiaxis toolpaths so bear with me lol. I figured this would be the best and easiest way to do this. Any ideas? I have a lot to program so the easier the better! In the past the company I work for has just surfaced them with decent results, it just takes about 4 hours per part!! Thanks, Jon

SAMPLE.MCX-7

[Peter - Avivi CNC Solutions]

Here is my sample, I used the new swarf TP, it rocks BTW...

And UnTrimed surfaces (from trianges) for drive.

Sorry for metric...

[JMahon]

Thanks buddy, that's getting me started. I see you said it was swarf milling tool path, but when I open it, it says its a "parallel cuts" toolpath. It also gives me this error message....

[?Mark]

Peter is running newer version. You need to update yours to see his toolpaths correctly.

[JMahon]

When I look at it under the operations manager, it says swarf milling. But when I open the parameters, it gives that message and comes up as a parallel cuts toolpath...?

It also doesn't let me view the geometry.

I see you untrimmed the surfaces for the walls, but what about compensation surfaces?

[JMahon]

Oh ok...gotcha Mark, thanks. I have been leary of updating from all the problems I may encounter...

I may update Monday morning.

 

Any other approaches? I know there are probably a million different ways to get it done.

[JMahon]

Alright, I updated and checked it out. That was pretty much exactly what I was looking for. Thanks Peter!

[JMahon]

Peter, I have gotten that toolpath to work for most of the teeth, but when I get towards the top of the part, it starts to not blend the surfaces. It just climb cuts each individual surfaces, starting from the left side...if that makes any sense.

[JMahon]

Heres my file...Its actually not doing what I want it to do at all anymore. I had it going good yesterday and now Im stumped...

Someone help please!!! Im stuck!

NEW SAMPLE.MCX-7

[Peter - Avivi CNC Solutions]

I set the cut direction to conventional, and voilá!

Or do we want climb? Hmmm...

[JMahon]

Ill give it a try at work tomorrow. I would prefer to climb mill if possible(stainless steel). I'm worried about burrs and finish as this is not going to be metal finished and these are medical parts.

[Peter - Avivi CNC Solutions]

I would prefer to climb mill if possible(stainless steel). I'm worried about burrs and finish as this is not going to be metal finished and these are medical parts.

OK, I got it. I fight then...

[Peter - Avivi CNC Solutions]

Sometimes the oldish swarf works also....

[JMahon]

I ended up using the new swarf. Went back to solidworks and removed one row of cuts, so there were just rows of cuts.

Thanks. I couldn't have done it without your help.

[Peter - Avivi CNC Solutions]

Your welcome!

Yes, lot of gaps were the main problem, wasn't easy to handle it, but you fixed it well then!

[Jayson Kramer]

Here is the file done using Curve 5 axis sir. let me know if this what you are trying to do?

SAMPLE-CADCAM.zip

[JMahon]

Thanks Jay, I will give it a shot when I get to work tomorrow! I am already making parts, but I would love to see a new way to get it done. This was my first 5 axis toolpath and I can really use some help. Plus I have 29 more of these to program!

[dan.w]

Hi there,

- I thought i would try and contribute something after learning from everyone else.

 

I looked at both solutions and combined them -

• I made a 3-pt arc across the base of the teeth for the bottom rail
  
• Multi-axis >> Tool Box >> Swarf Milling >
  
  • Wall Surface - Picked the faces with the solid selection and face highlighted
    
  • Bottom Rail - picked the arc at the base of the faces.
    

I'm new to the tool path but it looked liked it worked. You might have to play with linking to keep the tool down in the areas with slots and getting it to feed into and out of the part.

Seemed pretty quick to me.

 

Merry Christmas,

 

Dan

[crazy^millman]

I looked at the file and thought I would do it with a full profile custom tool. Another thought was curve 5 axis where you could spin the tool and do each tooth as a pass. Another thought was stand on it side again with a custom Made tool with the root and top in the profile done in one shot. Use do something like this for another company with a 8" dia x 12" long cutter. Since cutting this will take a lot of time, profile cut in one pass and done I think would be your quickest and cheaper way to machine this part. Can do it all day long with 5 axis, but I wonder why you are stuck on that process?

 

 

[JMahon]

I thought about a custom profile tool but with 10 different profiles and only 6 parts per profile, boss man doesn't wanna shell out that money. Maybe for production runs. How were burrs when you did the similar part? Tiny burrs are usually our main problem when machining these parts. They only get very light glass bead for finishing.

[crazy^millman]

Burrs are just like anything when you overlap you create the burr. Rough leaving .005 then come back and finish with .005 and would be a lot less burr. What would a tool cost you? You said 29 more to program are none of them similar where tools would cover some of the other ones? Can you make that suggestion to the customer? What is your programming time per part going to be making all 5 axis toolpaths? Profile cut and done. Index 90 degree profile cut and done. 5 axis toolpaths and time to run said 5 axis toolpaths where will you come out ahead?