advanced 3d carving on 4th axis rotary

Been practising some simulations in multiple different cad softwares such as fusion 360/artcam but the once thing i cannot do or find tutorials on how to do it is carve 3d hands on a rotary. i have seen maybe 2 at most on youtube of someone carving it with success but there is no guides on how they did it. here is what i am trying to simulate so if anyone has any tips i would really aprecia and i understand its going to take some skill to learn it.

edit.. seems the ones you can do it on are £500 a month subscription, the trial versions are standard and dont let you use the features so i am forced to either pay £500 a month to learn and probably find out its way to advanced for my needs or never try to begin with which is something i hate doing lol.

https://www.youtube.com/watch?v=rrk6wqcB54g

You can use an indexed 4th strategy rather than a rotary one, this will let you machine with the work fixed at multiple index angle intervals and access the entire part.
You can do this on a 3-axis system by having multiple copies of your part rotated in CAD to the required index angles and generating a path for each, paste the code together and manually add your index angles between blocks of code.
Ensure your clearance plane takes into account the rotating stock, it's easy to bust a cutter if the stock rotates and you haven't allowed for the corner height as it sweeps past! ;-)

never knew this was possible thank you,

You do need to get your part on-axis in CAD so you can rotate it in CAD in a way which will match your stock rotation on your 4th axis, if you hit any walls give me a shout! ;-)

Quote:

---

Originally Posted by magicniner

You can use an indexed 4th strategy rather than a rotary one, this will let you machine with the work fixed at multiple index angle intervals and access the entire part.
You can do this on a 3-axis system by having multiple copies of your part rotated in CAD to the required index angles and generating a path for each, paste the code together and manually add your index angles between blocks of code.
Ensure your clearance plane takes into account the rotating stock, it's easy to bust a cutter if the stock rotates and you haven't allowed for the corner height as it sweeps past! ;-)

---

This is really interesting as I am looking to do the 4th axis indexing as well using Aspire V9, I have just built an indexer and constructed a stand alone control for it to be able to move from cnc to miller when needed.
I am not looking to carve a hand but how you would construct the full code would be very interesting.

Phill

i will keep posted for anyone else interested because if i can figure it out then anyone can as i have no experience at all but i do love a challenge.

is it possible to preview a gcode made from deskproto?

Quote:

---

Originally Posted by reefy86

is it possible to preview a gcode made from deskproto?

---

Hi Reefy, I have been running with a demo of DeskProto today and it is producing a good Tap file but very large, so I have not got the tool-paths right yet some more testing required, I think it will do what you want and it's not too bad to learn.
Download a copy put an STL into it and watch the video for the settings you need.

Phill

Quote:

---

Originally Posted by phill05

Hi Reefy, I have been running with a demo of DeskProto today and it is producing a good Tap file but very large, so I have not got the tool-paths right yet some more testing required, I think it will do what you want and it's not too bad to learn.
Download a copy put an STL into it and watch the video for the settings you need.

Phill

---

The use of STL models for CNC path creation could be part of your file size issue, the paths will be following the polygons which form the surface and there will be many of them ;-)

Quote:

---

Originally Posted by magicniner

The use of STL models for CNC path creation could be part of your file size issue, the paths will be following the polygons which form the surface and there will be many of them ;-)

---

Nick I don't want to high-jack Reefy's thread but looks like we are both thinking along the same lines here, what would you say would be the best format to use to produce either a hand or in my case a car if not an stl.

Phill

Quote:

---

Originally Posted by phill05

Nick I don't want to high-jack Reefy's thread but looks like we are both thinking along the same lines here, what would you say would be the best format to use to produce either a hand or in my case a car if not an stl.

Phill

---

Phill,
You could process an stl to reduce the polygon count, meshes lend themselves well to complex shapes but if you have fine detail in a mesh model you have a huge number of small flat surface elements which will break CNC tool paths into hundreds of thousands of short straight moves.
Ideally you should work in the native format of the CAD system you use, then your CAM can use curves, I use Bob-CAD/CAM V25 so anything I want to share is usually exported as both .step and .iges and the recipient uses which suits them best, I only use the stl format for exporting parts for 3D printing.
Regards,
Nick

figured it out and now have the results i was after and feel comfortable with the software now so that's great but the problem i am having now is the total hours to complete 31 hours, the size is only 180mm in length and 51mm in height. It may have something to do with what you say about stl file but my model was done in 3ds max with turbosmooth so it has alot of polys

Quote:

---

Originally Posted by reefy86

figured it out and now have the results i was after and feel comfortable with the software now so that's great but the problem i am having now is the total hours to complete 31 hours, the size is only 180mm in length and 51mm in height. It may have something to do with what you say about stl file but my model was done in 3ds max with turbosmooth so it has alot of polys

---

What roughing cutter & path and finishing cutter & path are you using?

here is both rough and finish settings

Attachment 23491Attachment 23492

Why are you roughing with a ball nosed cutter?

no idea i am just following a tutorial that has similar details

Unless your stock is very close to your part size the limited DOC and greater cost of ball end cutters means it makes no sense to use them as roughing tools, was the tutorial authored by an industry professional?

This was the tutorial

https://www.youtube.com/watch?v=m8aWk6oTiF0&t=707s

Quote:

---

Originally Posted by reefy86

This was the tutorial

https://www.youtube.com/watch?v=m8aWk6oTiF0&t=707s

---

You could do the job quicker by roughing out to within 3mm of the finished surface with a more efficient cutter, then semi-finishing and finishing, provided roughing doesn't chip the material.

Did you notice that his spindle speed is 10000 rpm?

for now i have no idea what spindle speed my machine will be able to do once finished but changing spindlespeed in deskproto doesnt affect the machining time, as for the cutter i have no idea what tool is best used accept the ballnose that only gets shown in tutorials.

Quote:

---

Originally Posted by reefy86

changing spindlespeed in deskproto doesnt affect the machining time.

---

If your CAM doesn't do it then something which must be part of your workflow must change feed speed with RPM - for any given material/machine/cutter combination there will be a small range of Feed per Tooth values which will yield optimal finish, tool life and job time.

Use a Feeds & Speeds calculator to get a ball-park figure and refine that for your machine through trial and error, a job which runs with a given RPM and feed speed can be problematic at half the RPM, you will be asking your cutter, machine structure and work to deal with double the depth of cut per tooth with significantly increased forces on everything.

Quote:

---

Originally Posted by reefy86

as for the cutter i have no idea what tool is best used accept the ballnose that only gets shown in tutorials.

---

Even when you have 4th axis full rotary available it's common practice to rough out with an efficient cutter, a 3-axis tool path and indexed moves then semi-finish and finish with rotary because that's more efficient strategy for time and tooling costs.

HTH ;-)

Thank you, the more i play around with it the more i bring the total time down but i won't know for sure how well the detail and how smooth it is until i test on the machine.