Constant scallop

[Micromoldmaker]

I've been trying to use MC's surface finish constant scallop to get the kind of toolpath WorkNC calls Constant Z-Level finish. The results haven't been inspiring; the processing time is pathetic and when I run the program on our Mori Sieke I get feeds of between 2 IPM to 20 IPM of my programmed 50 IPM. What I liked about MorkNC' constant Z-level toolpath was the consistency of tool scallops and the great finish.

Any hints or suggestions?

[mayday]

have you tried finish project blend?

or do a 2d pocket with constant overlap and project that nci onto the surface model

[PE @ IHS]

Scallop is not the right toolpath for a constant Z level finish. Try Project blend as stated above, or finish contour with the shallow option turned on.

 

If you put a file on the FTP, it would be a lot easier to make suggestions.

 

Is your arc filter turned on, and is it set to 2:1?

[cadist]

The reason your feed is droping could be with arc filter. But scallop is definitely not constant z toolpath. If you want to compare mc toolpath to worknc then I would recommend you put your file on ftp. and let forum member prove this.

[Micromoldmaker]

I placed the file here: ftp://www.ppcadcam.com/Mastercam_forum/MC...es/INS_A_NC.MC9

A clarification: the WorkNC toolpath I was so fond of was actually called "3D Drive Curve Finishing," which you can see on this page:http://www.sescoi.com/sescoi.nsf/wnc_finishingtoolpaths.html?OpenPage&charset=iso-8859-1

[PE @ IHS]

Try project blend with the outside boundary and a point as your drive curves. I believe this is the closest thing to what you are trying to achieve. Turn steep wall support on.

[Richard Thomas - Mastercam UK]

One reason for the varying feeds could be that the post processor is setup to output feeds in Inverse Time rather than your programmed feedrate. I could be way off here, but it's one thing to check for. Unless you know for fact that it isn't using inverse time, check with your reseller, or the people who originally supplied your post processor.

[P_Scott]

MICROMOLDMAKER,

 

Mayday and Peter Eigler are referring you to the Surface-Finish-Project-Blend 3D toolpath in Mastercam. This is equivalent to the toolpath you linked to for WorkNC. The Finish-Project-Blend toolpath is designed to use defined contours to produce parallel toolpaths and then project those parallels onto any surface shape, maintaining the cusp, or scallop height on those surfaces. The parallel contours can be linear, circular, splines, or closed for one and a point for the other. The Project-Blend toolpath has almost unlimited use in application. Constant Z machining is analogous in Mcam as Surface-Contour toolpath, which will machine surface boundaries at one depth per pass, then transition to the next depth of cut. This resembles a Civil Engineer's map, with the differences in height being toolpathed as closed contours around the surfaces. HTH

[Micromoldmaker]

Is there a surface-finish-project-blend 3d sample file that came with MC? I don't see it in my install. Has anyone uploaded one to the ftp site?

[Jan Bohman - AME AB]

Micromoldmaker,

 

Look in the samplesproject folder. There are simple examples for all the "project" functions.

Project Blend is what you are looking for.

 

/Jan

[Hardmill]

quote:

---

The results haven't been inspiring; the processing time is pathetic and when I run the program on our Mori Sieke I get feeds of between 2 IPM to 20 IPM of my programmed 50 IPM.

---

1. Why don't you put your file on the ftp site.

2. What kind of control is on your Mori??

3. If the processing time is slow you should upgrade

to Maint. Z-level processing is much faster.

What ver. are you using???

 

 

PEACE

[Reece L Gibson]

How old of a Mori are we talking here? What's the control? Lot of the older controls would decel on end points through the controls software.Might be data starvation.

[Micromoldmaker]

"1.Why don't you put your file on the ftp site.

2. What kind of control is on your Mori??

3. If the processing time is slow you should upgrade

to Maint. Z-level processing is much faster.

What ver. are you using???"

 

 

1:ftp://www.ppcadcam.com/Mastercam_forum/MC9_files/INS_A_NC

2::Mori NVD5000 (less than 2 years old)

3: MC v 9.1 SP.2

 

 

I tried using surface-fin-project-blend 3d but haven’t gotten anything satisfactory.

[Thad]

quote:

---

3: MC v 9.1 SP.2

---

Maintenance? That's where the improved crunch time is, IIRC.

 

Thad

[Hardmill]

quote:

---

2::Mori NVD5000 (less than 2 years old)

---

What control??

 

I can look at your file tonight, unless you want

e-mail it to me.

I got limited internet access at work.

 

 

PEACE

[Micromoldmaker]

The control is FANUC, whatever the latest version is. (Do they ever change?)

Hardmill: I sent you the file by email. This is the best I've been able to with fin-proj-blend 3d.

[Midwest]

 

 

1.Scallop with a larger ball em and a leftover tool path with your 1/16 ball.

[Hardmill]

I'll take a real good look at it at home.

From past experience(and I also work in a mold shop)

Your never going to get good results on any given

3D senario using just one toolpath.

The vast majority of my molds get at least 2-3

toolpaths on them.

I'm thinking I'd use a combination of surf-fin-contour

and surf-fin-scallop.

I'll get back to you later.

 

 

PEACE

[Müřlıń®]

quote:

---

Your never going to get good results on any given

3D senario using just one toolpath.

The vast majority of my molds get at least 2-3

toolpaths on them

---

+1000 to Hardmill

[Hardmill]

MICROMOLDMAKER,

Check your mail.

 

 

PEACE

[Micromoldmaker]

Hardmill-

I checked my email; are you sure you have the correct address? I did not receive anything. I'll send you an email so you have a return address.

[Hardmill]

Check again

 

 

PEACE

[Micromoldmaker]

Must be having server problems. I'll try again later.

Thanks for your help.

[Brad St.]

Micromoldmaker, just some quick suggestions for you.

 

1) (roughing) multisurf rough pocket

2) (semi finish) multisurf parallel 45 deg twice at a + & then - angle cut.

 

here comes the twist:

3) (finish upper walls with a coons patch top to bottom, to the bottom of the fillet) Coons patch.

4) (finish floor) multisurf parallel the floor using a direction that is either parallel to the length of the part or perpendicular. If you can, containg the floor with a boundary and offset it to .002-3" inside to keep the tool from hitting the corner fillet. The small gap could be pick out later if you feel it's needed with a 3-d contour.

 

There are otherways to get the walls to finish down but it would at more steps in the program (not a bad thing just more to explain). Coons works nice if you know how to use it and filter it correctly.

 

Leave stock accordingly as you deem it necessary for your tooling and machine to get a good finish.

 

p.s. I hope you know what a coons patch is, not really used nowadays but I've cut mannnnyyy a trodes in my time with it. I think it's still very usefull. If your not carefull in defining your geometry, your tool will deviate from the norm.

 

Best Regards, Hope this helps

[foolsh]

a coons patch?heard of it but don't know how to use it,only wireframe used so far and easy to use is the 2D swept