Tool paths on letters help - getting the best edge inside tight corners

[Butcher84]

Sorry for the title but im unsure how to word my problem



I have recently started using a CNC machine at work the company i work for bought a new machine sent 3 people on a 2 day course and expected them to come back with 10 years of knowledge, so we currently have a CNC machine with zero experienced staff running it, we have basicaly stumbled our way through after the 2 day day course.



Our boss wasnt happy with the corners on the text saying its too rounded, So i worked out a way out of getting round it but im hoping someone can suggest how i do all this in Alphacamm, i currently duplicate the letter in VCarve Pro then cut it up and leave a small line to put the tool on before the finish pass import it into alphacamm and add the tool paths (See pictures below)



Path 1 - 6mm tool leaving 0.2 stock

path 2 - 1.5mm tool to get into the tight corners at finish size
path 3 - 3mm tool to take to finish size and give a nice edge.


The reason i dont just add path 2 all the way round the letter is becasue the tools are very weak they snap very easy being only 1.5mm thick and it cuts the time down massivly as 1.5mm usually set to 3 passes
Im starting to look outside of my comfort zone and push my limits, iv been looking into adding all my paths to a tool path (like a group) so when i add my path its adds them all. but the current way i do this doesnt work as sometimes it decides to put path 2 inside the edge sometimes outisde the edge for the tight corners

Attached is 3 pics showing you my letter with the passes i have and you can see the small line i leave (same for any letter with a tight corner)

Any help greatly appriciated!
　

Similar Threads:

• Need Help!- Tool paths all weird. Highly infuriating. Explaination inside.
• Cleaning up inside corners on profile toolpath
• Probing inside corners with the 2010 Screenset
• Inside Square Corners
• Milling Tight Inside Corners???

[ger21]

How deep are you cutting? If it's 6-8mm or less, just use the 3mm tool, and make 2 passes, followed by the 1.5mm tool?

[ger21]

And tell you're boss, if he wants an AlphaCAM expert, you'll need about 30 days of training, and years of practice.

[Butcher84]

I have he wont listen, never will! 2 people have already plunged the head through the bed and one twisted the arm so bad it jumped 50mm off the runner on the left, id be surprised if it lasts a year, I enjoy learning the machine but they haven't given me any avenues to learn from seasoned pros this and youtube is my mentor!

I have tried that before but he didn't like the step it left (there was no step but slightly more polished where the 1.5mm starts and finishes. should i be using lead in edges for that kind of thing? can i apply a pass onto a line and then trim down where the tool will cut to only cut the 'V' parts (like the pic)

Thanks for your help guys!

[ger21]

Try cutting the entire letter with the 3mm tool, with a 0.25 offset, then clean up the corners with the 1.5mm tool, again with a 0.25mm offset. Then a full finish pass with the 1.5mm tool. That should give you a consistent finish all the way around.

[Routerfiend]

Hi
I See your problem and your boss is unreasonable. He may have paid for training but that only goes so far. I had a couple of hours training 15 years ago and have learned by trial & (alot of ) error. Over time you get to grips with it but alphacam is such a huge programme you can`t learn it all in such a short space of time.

Using the smallest cutter (1mm ) you will still end up with a 0.5mm rad in the corner. See attachment. The only way to get it to come to a point is to use a "V" cutter but at that depth you will still have a problem as the deeper you cut the wider the cutter becomes.

You can use a "V" cutter if you use 3-D engraving and get into a point but it depends on your letter style ( See other attachment ).

What material are you using ? And what machine are you doing it on ?

I tried to upload the alphacam .ard file but the zone wouldn`t let me so the screen shots will have to do. Sorry you`re having a tough time but stick at it . It will come with time ( and alot of frustration)

By the way the straight cut is a helical cut. It`s a bit kinder on the smaller cutters just make sure you set the pitch to about 0.35 and cut your feed rate.

Syd

[RCaffin]

Hehehe
Plead ignorance and ask your boss to show you how to do it.
Yeah, he is an idiot. You will have to figure out two things: how to get a satisfactory result and how to manage your boss. The latter is harder.

Cheers
Roger
PS: the V-point cutter is a real option, but programming it will be difficult for a novice.

[FrankCNC]

Hi,

The method I use for sharp corners in letters is either a V Carve type tool or small Ball Nose using AlphaCams Rough or Finish with Sloping Sides, the attached .jpg should give you enough info, this works in machining metal plaques not sure if it will work in wood, also set Tool Directions to Outside of the Geometries.

Regards.