Milling glitch?

[Thad]

quote:

---

I'm with the others here. It's not a glitch. You need to use a surface toolpath. If you'd liek to have that functionality resident in the 2D Pocket toolpath, you'll need to send in a request to [email protected]. What you are requesting requires 3-D Compensation and Pocket only offers 2-D.

---

James,

 

I'm glad you jumped in here. With another opinion, maybe I can figure out why I'm not getting my point across.

 

What is it about my simple 2D pocket that requires a surface toolpath?

 

If I program to cut a 3" square pocket leaving zero stock and the pocket, when finished, measures 2.867 square (because I used a 1" bullnose instead of a 1" flat bottom), I'd call that a glitch.

 

Thad

[Thad]

Andrew,

 

I appreciate your thought on this, but I don't know what "Constant Surface Speed for milling" is. I'm living in a 2D world here.

 

Thad

[McRae]

Thud,

 

This is not a "Simple" pocket. You are describing something that has a truncated radius and Mastercam would have no Idea that there existed a radius here as we only define a chain of edges with no other properties to define it.

 

What you are looking for is a roll around corners type of toolpath that would for example place the tool in a modified radial position based on the corner radius and depth of cut. If you proclaim that Gibbs will do it, then I say "Yeah - Buy Gibbs for all your trival, Low Ap(Depth of cut) with Big Corner Radius tool pathing needs..."

 

If the radius is a full radius and the tool didn't do what you want, then call Johnnie Cochran - you have a case - Glitch, Glitch, Glitch!

[McRae]

OOPS - I meant Thad!

[Guest CNC Apps Guy 1]

quote:

---

What is it about my simple 2D pocket that requires a surface toolpath?

---

Thad, you're asking for 3-D tool compensation on a 2-D toolpath! The toolpath not only needs to comp for diameter but for depth due to the cirner radius.

 

What I did was create a rectangle 2x2 then create a pocket in in the center 1x1x.0625 deep. I created a solid with the 2x2 rectangle. I extrude cut the .0625 deep pocket. Then I created the .250 fillets on the 4 vertical edges, then created the .125 fillet on the bottom face.

 

Do a Pocket toolpath in there chaining the geometry you used for the extrude cut.

 

Backplot it and you'll see what I mean. It is comping correctly for the toolpath. If youn need more compensation options, you need to select a surface toolpath.

[gstephens]

quote:

---

I don't have the time or the energy to get into a pissing contest with you. Thank you for your input.

---

WOW! I've been told to shut-up and mind my own business! Sorry...no can do. Seeing as how I teach this stuff, I try to add my input so that others might see how things can be done in a different way. I also do my best to defend Mastercam from bulls**t, which is now the only reason I'm still trying to get through to you.

 

I think I FINALLY see what the problem really is.

 

The print shows the 2-d outside boundary of the top of the pocket (which is at some section in the middle of this .250 corner radius). Apparently it's too difficult to actually DRAW the lower tangency (from which the 2-d toolpath can be easily created using my previously posted methods).

 

Here's how to do it:

Create a rectangular surface at Z-.08 bigger than the pocket (I know you're only using Mill level 1, but you CAN create surfaces just not machine them). Create a surface fillet curv/surf selecting the flat surface and the chain of the outside boundary of the pocket. set the radius to .25. Go to the options for the fillet and create only the rails. Do it.

 

Chain the bottom rail for the pocket routine and use -.25 stock to leave.

 

Does this work for you? I've now given EXACT step-by-step instructions for getting this toolpath using 2-d pocketing WITHOUT having to do any "extra calculations". I do apologize that you have to actually do some extra geometry creation, but refer to my previous comment concerning software limitations.

 

If you still don't believe that this will give you the toolpath you're looking for, I'm sorry but I can't do anything else for you (nor do I believe anyone can). Try it anyway, and do it in the same file as the one with "extra calculations and such" that give you a good part. Verify both toolpaths together and see if there is any difference.

[Guest CNC Apps Guy 1]

It doesn't get any simpler(is that a word?)that that....

 

JM2C

[BernieT]

Mastercams support for bull nose tools is fairly recent and was developed for use only with surfaces. (I believe) Jim is right, Thad, you are doing 2D toolpaths and expecting 3D results. Ain't gonna work.

 

BerTau

[iowajim62]

Thad,

Wouldn't it be easier to just go into Side view

and extend (draw fake geometry) the .25R up .17

more and then go back to Top View and draw some

new pocket walls at the top of the extended Radius? I know you don't wanna draw extra geo

but it would be done already and you'd be working

on something else. As far as limitations go, I say

do it anyway you can. My boss doesn't wanna hear

excuses like, "The software has limits for this

kind of Cut" he just wants it done.

Jim

[Thad]

Thank you all for your input.

 

Thad

[Rekd™]

Thad,

 

I understood your situation from the first post. Only because I have to deal with it on almost daily basis with GibbsCAM. I'm fairly fluent with mastercam, and don't recall that option being available in normal 2d toolpaths.

 

GibbsCAM on the other hand, does it no matter what. Very VERY frustrating. Especially when using CUSTOM tools. I am constantly having to lie to get the results I want. Idealy, it would be nice to be able to turn this kind of option on or off. ( I would leave it off for ever!)

 

It can be a nice feature in GibbsCAM, but as I said, it's VERY frustrating having to deal with it the OTHER 98% of the time I don't want to use it. I wouldn't be surprised if the wise folks at CNC had already looked in to this, and smartly decided against it...

 

-Rekd

[McRae]

Ladies and Gentlemen, Thad has thrown down his weapons and is laying on the floor clutching his head saying "Why don't they understand... "

 

Thad, I agree with your statements that the software doesn't compensate for the axial depth of cut amount. I do not share the opinion that it should.

 

Webmaster - Please attach the lock now.

[Guest CNC Apps Guy 1]

I don't think there was ever(well, maybe for a post or two) in doubt that MC was not comping. The debate seems to be weather it belongs in a 2D toolpath (Pocket) or not. I believe that this should remain the same as it is now as well.

 

JM2C

[Rekd™]

James..

 

Are you sure that's not Multax??

 

-Rekd

[TheePres]

Thad,

I didn't read thru all posts on this thread, but I understand the problem you are describing about no compensation for shallow cuts with bull or ball nose endmill. I ran into this situation also when converted to MC from UG, my workaround is to create offset charts for different radii and rely on them often when drawing my geometry creating false (tangent) lines for actual toolpaths. In UG if you had say a pocket with outward beveled walls, I could select topmost edge for driveline and select floor depth and Ug would automatically compensate regardles of chamfer/form tool diam. Sorry to all, not meaning to knock MC which I still consider overall far superior. Just a neat feature i miss.