[FoxCNC1]

I modeled this part in inventor and I am going to be doing the programming in aspire.
I am unsure how the make the ramp of bevel.

Here is a section of the part.

[FoxCNC1]

Here is another example. My question refers to the sloping plane.



The only way that can think of doing this in aspire is to bring in the 3d model in the 3d environment and do a rough and finish pass. The challenge for me is that just like the first example I posted, the part is mostly a 2D part with the exception of the slope.

I am wondering if the only way to do this sort of 3D carving / CNC will by creating a 3d model and using the 3d tool paths.

[ger21]

Bring in the 3D model along with your 2D drawing, and make sure they are aligned. Create a closed vector around the ramp area only, and just do the rough and finish passes inside that vector.

Then cut the rest as you normally would.

[FoxCNC1]

I will try that. Will I have to change my to a ball end to do the ramp?
I want to make this part out of clear acrylic and have bought a "special" plastics bit from Amanatools to do the pockets and 2d cuts. I am wondering if I need a different bit for the carving and if you can please recomend one, or just steer me in the right direction.

thanks you.

Here is a link to the bit I purchased:
Solid Carbide Spiral Plastic 'O' Flute -ToolsToday.com- Industrial Quality Solid Carbide Bits

[ger21]

You can do the roughing with the Amana bit, but yes, you'll need a ballnose for the finish passes on the ramp. I'd just use a 2 flute 1/8" or 1/16" if you need to get closer into the corners. Make sure the ballnose is sharp.

[Tkamsker]

Try madcam or bobcad ...or rhinocam

Gesendet von meinem SM-N9005 mit Tapatalk

[Robert M]

Hummm...To each it's preferences....but too many insatisfaction stories about BobCam to my taste to suggest it !!
If you have a legit Inventor licence, simply apply to Autodesk CAM solution (see here)....it's free for Inventor users.....and it's MUCH better then MANY others.
BTW...it's 'do-able' in Aspire....just like some others CAMs that handles 3d !!
Good luck.... ;-)

[FoxCNC1]

Thank you Robert,
HSM for inventor doesn't do 3D.

[Tkamsker]

Yes insatisfaction but ...
If you can t afford mastercam or sprutcam Then ... what is a True Option ? If you use rhino and dont have a lathe rhinocam could help

Gesendet von meinem SM-N9005 mit Tapatalk

[simracn]

You can do the roughing with the Amana bit, but yes, you'll need a ballnose for the finish passes on the ramp. I'd just use a 2 flute 1/8" or 1/16" if you need to get closer into the corners. Make sure the ballnose is sharp.

Not sure of the amana part number, but in onsrud, good plastic ball nose is 52-200b/bl for soft and hard plastics and 65-200b and 300b series for soft plastics the 65- series is 2 and 4 flute depending on your needs. I do quite a bit of cutting in cast plex and prefer the onsruds and the O flute, but amana is a good brand, less expensive :-)

[FoxCNC1]

I did a quick goggle search and came across 2L inc.
I ordered

PWB2-0625-2 - 2 Flute, Ballnose End Mill for Plastic/Wood, .0625 cutter dia., .250 shank dia. x 2.0 OL
PWB2-125-2 - 2 Flute, Ballnose End Mill for Plastic/Wood, .125 cutter dia., .250 shank dia. x 2.0 OL

To try out. The The bits were 20 dollars each, I could not justify the $45 for the amana tool variation.
I think they should work fine for general 3D stuff.

@simracn, in your opinion, what qualifies a bit, a good bit for plactic ?

[simracn]

Hi Profoxcg,
Main thing is sharp and then the tool grind, such as the 'O' flute. It helps evacuate the chips. I think those a the two most important when looking for plastic/plex bits. I normally climb mill when doing plastic, conventional has more of a tendency to 'weld' the chips back to the material you are cutting. One other thing i like to do on edge cuts, is do a rough pass and then a finish of about .020 - .040.
Try to find bits specific for plex/plastic. A cpl of places is MSCdirect.com, they have some decent prices and selection. Another is precisebits.com in Colorado. If you are using a trim router or even some of the bigger router motors, they produce precision collets, nuts and accessories. Tool bits, from two and 4 flute to diamond ground for composites and i think good prices as well on their products.
My normal speed is about 14-18000 rpm, the smaller the bit, the faster you want to go. Dont know if you have the chip load formula, but it cant hurt to pass it on feed rate = RPM x # of cutting edges x chip load 72 IPM = 18000 x 1 x .004 But also remember to consider the rigidity of your setup and machine. On my small shark i try to keep my feed at about 40ipm, at 16000 rpm with a 1/4" bit and no more then .100 to .125 deep at full width of cutter.
Dont know how big your shop is, but if you start smelling hot plexiglass, VENTILATE OR WEAR A RESPERATOR know from experience, the fumes can knock you on your butt!
I know a bit long winded, but thought some of my experiences may help others as well. :-) And hope it answers your question Profoxcg

[FoxCNC1]

I appreciate that, thank you.
Why does a smaller need more speed (rpm) ?

[simracn]

smaller bits are more fragile, and need a lower chip load to keep from breaking as easily. mainly talking about under 1/8" is where it starts mattering more. Onsrud has a good place to start for chip loads here Chiploads | Feeds and Speeds | Metal | Plastic | Composite | | Documents if you dont have the exact bit, look for something close to give you a starting point.

[FoxCNC1]

smaller bits are more fragile, and need a lower chip load to keep from breaking as easily. mainly talking about under 1/8" is where it starts mattering more. Onsrud has a good place to start for chip loads here Chiploads | Feeds and Speeds | Metal | Plastic | Composite | | Documents if you dont have the exact bit, look for something close to give you a starting point.

Thank you, I understand.
I think the most important piece of information is to have the chip load from the manufacturer from your bit and plug it into the formula. - right?

[simracn]

Yes on the mfg's numbers into the formula, and adjust from that starting point if needed. You get better with more experience :-)

And i like to say the only stupid question is the one not asked ;-)

[FoxCNC1]

thank you.