contouring

[skit]

I recently wrote a program to machine a internal

hemispherical mold half.I used toolpath/contour

to do it and it worked fairly well with two exceptions.One is that this method will leave a

xxxx at the bottom center of the hemisphere.The other is that the surface quality diminishes as

the ballnose gets closer to the bottom.Do any of you mold makers or anyone have any suggestions?Thanks!

[Lumpnut]

quote:

---

will leave a

xxxx

at the bottom

---

Easy there Skit , this is a family friendly forum round' here'.

 

Post the file on the FTP if you can. That way more people can have a chance to help you out. If you cant , You could e-mail it to me and I could look at it in a bit.

 

What version of Mcam ya runnin ?

 

[mayday]

depends on the shape. maybe try scallop or parrallel or project blend. in contour you may need to enable the shallow and flats option to get the flat area's

 

hit alt-c

run the tpcfg c-hook and turn on the options

[polishman]

I think we call it a TEAT?

[HevyMetl]

I if there are any surfaces below 20°'s of horizontal I always follow up with secondary operation of Surfacefinishshallow. This tends to cleanup all of the uncut material left by the constant Z toolpath. Scallop works will but it will tend to have minor z movements and transitions during the operation making the coded file much longer.

[Chris Rizzo]

do what MayDay says.

 

There's a check to add cuts to shallow surfaces in contour. Even so, contour is'nt great for shallow surfaces. Maybe add surface>finish>shallow to clean up areas >20 degs or so.

[Hardmill]

quote:

---

Do any of you mold makers or anyone have any suggestions?Thanks!

---

No one toolpath is going to get it all.

For core or cavity I always use at least 2 diff. toolpath. ALWAYS.

You'll pull your hair out trying to do it with one toolpath.

 

PEACE

[g huns]

Speaking of no toolpath doing it all... I posted a file on the ftp in called cashew gate.mc9. I cut lots of these and was wondering if anyone knows a better way than what I've got. I already got these done so it's no big deal. Just not so happy with the results that surface-finish-contour gives me. For the bottom of the countour to look decent I have to get way small on z steps(.0001) and it takes about 15 minutes to cut each block. Would checking the boxes for shallow and flats help? Anyhow if anybody's bored I'd appreciate the input. Thanks.

[Rob Peirolo CNC Software]

Skit,

I believe the reason that the surface quality diminishes at the bottom, is because the point of tangency of the surface you are cutting and the flutes of the tool is getting closer to the centerline of your ball mill thus reducing the surface footage at the tool-work piece interface. Remember the formula S.F.M = (R.P.M.*Dia)/3.82.

My suggestion would be to step up the R.P.M. near the bottom. Also you could up the feedrate to keep the chip load constant.

 

Hope this helps

Rob

[HevyMetl]

Ignore the shallow and flats option in contour toolpath and run a second operation called surface finish shallow. Set the parameters to cut up to a 30° wall and cut it to run collapse. with your step over set to .0015 with a 1/16" ball end mill. This basically runs a scallop toolpath limited to surfaces under 30° form horizontal. It will clean-up the big steps left from the constant z motion of the contour toolpath. I use this strategy all the time for cores and cavities with great success.

[HevyMetl]

G Huns,

 

 

Check the FTP under cashew-gate-jj I added a second group on how I would cut it.

[g huns]

Thanks, I'll check it out.

[mayday]

quote:

---

You'll pull your hair out trying to do it with one toolpath

---

that had to hurt for a spin top like you.

[Micromoldmaker]

ghuns-

I placed a file called "CASHEW GATE_MICRO" in the ftp site. I find this to be a simple and straightforward way of cunning runners, gates and also cavities. As you can see I built a vertical surface of about .005 around the perimeter of the surfaces being cut to make sure the tool never rolls over the parting line.

[Müřlıń®]

Radial workes good on spheres where only one toolpath is wanted.

[g huns]

Thanks, what folder is it in?

[Imtiyaz Ali]

I can't upload mastercam file. but after reading your situation, I suggest Scallop is best alternative. here.

HTH

[Micromoldmaker]

Sorry. I thought I'd had copied it to the mc9 folder. Apparently not. And I have already erased the copy on my dektop. What I do is this: create draft surface .005 vertical on runner and gate surface perimeter. Mill rough parallel; finish parallel at 45 deg and another finish parallel at -45 deg. If you use a boundary to contain the toolpath it should work out just peachy.

[HevyMetl]

Ali,

 

Scallop does work well, but if you zoom way in on the back plot you will often see many small movements. This will kill a machine using HSM and look ahead. Our Makino running contour and shallow will destroy the time it takes just running a single scallop operation.

 

OFF TOPIC:

 

If I program the same scallop toolpath in Proman though it will run great. It just takes too long to use Proman. I guess there is a difference somewhere in the algorithims that Pro and CNC use to create toolpaths. I know you are a proficient Pro user from Cadist stated in your welcome. Do you have any ideas into this?

[Mike Mattera - TFM]

Create the XY circle and then the XZ 1/4 arc of the circle and use.... Toolpaths - Nextmenu - Wireframe - Swept. Works for Level 1

 

Mike Mattera