Radial toolpath

[david b]

I machined a shallow round dish,using a Dia 10mm x2.5mm rad cutter using the radial method.

What happend is the tool gouged and only gave me the correct form shape in th centre along x axis.I cut another one same method with a 10 ball job was good.So my question is can't MC do this type of tool path with a bull cutter??????It was like it did not take into acount the trailing edge of the tool.

 

 

thx in advance

[Allan]

Was it all one surface? I've seen Mastercam do strange things when a single surface has a dip in Z big enough for the cutter to get in. This type of surface does not happen very often in the cad world, but when using revolved surfaces you can have trouble. Try spliting the surf and see what happens.

 

You should let qc at cnc software know if you suspect it to be a bug.

 

HTH

 

Allan

 

EDIT

I've tried to recreate the problem and I can't. What version are you using? Can we have at the file?

 

[ 07-29-2003, 12:12 AM: Message edited by: Allan ]

[Müřlıń®]

DID the gouge show up on STL compair??

 

 

Murlin

[david b]

I uploaded the file to the FTP site under MC9_FILESDISH.It does show the gouge in verify.

 

 

[Thad]

quote:

---

It does show the gouge in verify.

---

Tsk, tsk.

 

Thad

[Jack Mitchell]

quote:

---

Tsk, tsk.

---

Thad is being a little coy with his response. at least I think he is.

 

NOTE: Verify doesn't trick or lie to you - verify shows the end result (almost too accurately - multiple crashes as well). Has anybody else witnessed layed crashes? - Bet your life on it.

 

Cause it's all math anyways.

 

Regards, Jack

[david b]

yes i should have verified before i cut it.

still doesn't answer the question.can MC caculate this correctly with a bull cutter.

makes me wonder if a shallow cutter path with a bull cutter would do the same thing and gouge.

[crazy^millman]

I am not sure where you created your infomation but you have a bad solid face. I did and an analyze of the solid at it show 4 bad contious face and you might want to go look at your setting in your tolerances in the setting and make sure it is set tight enough to reflect your machining and system tolerances. If you are using an outside modle program make sure it is set to the same as you are doing in Mastercam.

And yes it will radial toolpaths with a ball tool no problem I would also set my gap settings to 1 percent and make sure the check for gouge is checked. I would also follow the surface in this type of part. I have found it works best in complex parts and flat parts you have the other choices that work well.

Good luck and hello from the world up here.

 

[ 07-30-2003, 01:12 AM: Message edited by: Millman^crazy ]

[Fig sign]

David !

I put in the same folder corrected file Dishiskander.mc9.

Have a look .

I think you`ll understand what I`ve done !

 

 

Iskander s!z What you gonna put in teh dish ?

[McRae]

Dave,

 

MC doesn't handle curved surfaces with bull mill mathematics very well. When you point this out to them, they will say that your geometry is wrong and that you should design you part like this....

[Müřlıń®]

quote:

---

MC doesn't handle curved surfaces with bull mill mathematics very well

---

I would have to say this is correct.

 

After redrawing the part with arcs and lines, the radial toolpath still gouged....

 

 

Murln

[McRae]

Send the file to [email protected] and let them figure out why it doesn't work.

[McRae]

Create the surface at the bottom with a minimal amount of draft - .05 degrees or something. This way there shouldn't be any mathematical flip as the slope at the bottom never approaches zero and this chould keep the cutting action on the radius of the tool rather than at the tip.

 

See what I mean about the suggestion to make the software work is to change your geometry...

 

[ 07-30-2003, 11:37 AM: Message edited by: Andrew McRae ]

[david b]

quote:

--------------------------------------------------------------------------------

MC doesn't handle curved surfaces with bull mill mathematics very well

--------------------------------------------------------------------------------

Ok guys thx for the replies.

Tell me would you stay away from programing shallow curved surfaces with a bull cutter?Or stick to a ball?The bull would be a much better option but now im not to sure if i should risk using a bull on these types of surfaces.

 

 

Andrew----have you sent anything to QC?and do you get a reply?

 

[Müřlıń®]

If the reason you want to use a bull is because of the decrease in machine time, then use it with a rough pocket. And use a ball for the finish pass.

 

I cant think of anything I would want to cut with a zig-zag revolved using a bull.

 

Maybe graphite or plastic. Ramping down with a bull in a hole is not desirable.

 

 

Murlin

[Fig sign]

+1 for Murlin !

And one more case - you sometimes will not get the right dimensions the bull geometry can limit it.

BTW , David ,have you seen my file !?

I do agree with Millman^crazy ,you solid geometry is not clean!

And you have a gap between solid and surface.

And in advanced setiing you have roll tool between all edges thats IMHO a bad idea .

I don`t want to discuss if it is a bug or no,

may be not,cause your solid geometry is uncleen.

But I built a new geometry one revolved surface and there is no undercut now!

Personally I will mill it surface rough pocket with a hog mill,surface finish contour with filtering + shallow with a ball , far less code and time with a good result ,IMHO.

I rarely use radial toolpath .

I prefere surface contour less code and better tool cutting conditions.

 

Iskander lost between teh world up here and down there .

[McRae]

quote:

---

Ok guys thx for the replies.

Tell me would you stay away from programing shallow curved surfaces with a bull cutter?Or stick to a ball?The bull would be a much better option but now im not to sure if i should risk using a bull on these types of surfaces.

 

 

Andrew----have you sent anything to QC?and do you get a reply?

---

I have not sent anything for your specific application here but I sent a sample where this melts down in a Flow5ax path to my dealer. They didn't solve the problem, but agreed that it does happen. Shallow curved surfaces will work alright, it is when the surfaces become flat (zero slope - the tangent point on the cutter disappears and the system becomes indeterminate) that the software doesn't have the conditionals to support this. John Summers at Mastercam might have more insight into this - He and I had discussions last spring with respect to this stuff.

[david b]

plasttav i did see what you did thx.

the customer requested that i cut it with a radial toolpath using a bull and he supplied the geometry.It was from surfcam.