What's new
What's new

trochoidal single Z-20 AISI 304

cax

Plastic
Joined
Oct 3, 2012
Location
Italy
Hi guys I'm new in this forum this is my first post I'm Italian and I am in NC programming using Catia V5R21 principalamente.
I post a problem I work steel AISI 304 overall dimensions 450x250x20 mm (the quarry is 50.05 mm) you can run a trochoidal a single Z in the figure object with a sharp cutter Ø 16 to 6?
How can I get a software process performance?
Sorry for my english but it is translated by googletraslate
CAX
 

Attachments

  • troc.jpg
    troc.jpg
    42.5 KB · Views: 190
I would do something more like this:

xOnwu.png
 
Your path has A LOT of G1 moves in addition to the G2 and G3.

There are tons of software packages that will do various things with the toolpath. For your reference, I posted an image of Gibbscam with Volumill plugin. Just an FYI.

Your path may or may not be just fine. Good luck.
 
Hi,
a powerful tool path should be:
Example:
N10 G3 X13.6 Y41.303 I.4 J0
N11 X13.6 Y41.995 I-.2 J.346
N12 X13. Y41.649 I-.2 J-.346
N13 G1 Y40.649
N14 G3 X13.6 Y40.303 I.4 J0
N15 X13.6 Y40.995 I-.2 J.346
N16 X13. Y40.649 I-.2 J-.346
N17 G1 Y39.649
N18 G3 X13.6 Y39.303 I.4 J0
N19 X13.6 Y39.995 I-.2 J.346
N20 X13. Y39.649 I-.2 J-.346
N21 G1 Y38.649
N22 G3 X13.6 Y38.302 I.4 J0
N23 X13.6 Y38.995 I-.2 J.347
N24 X13. Y38.649 I-.2 J-.346
N25 G1 Y37.649
N26 G3 X13.6 Y37.302 I.4 J0
N27 X13.6 Y37.995 I-.2 J.347
N28 X13. Y37.649 I-.2 J-.346
N29 G1 Y36.649
N30 G3 X13.6 Y36.302 I.4 J0
N31 X13.6 Y36.995 I-.2 J.347
N32 X13. Y36.649 I-.2 J-.346
N33 G1 Y35.649
N34 G3 X13.6 Y35.302 I.4 J0
N35 X13.6 Y35.995 I-.2 J.347
N36 X13. Y35.649 I-.2 J-.346

in this way the cutter does not strain much......
 
The path i posted does the same thing. Take note, the first thing it did was do trochoidal toolpath to remove the center portion, just like your toolpath. It then takes advantage of radial chip thinning, and quickly removed thin amounts of material from the walls, which also keeps cutter strain to a minimum.

I programmed that to cut 4500rpm, 1mm width of cut, ~3000 mm per minute feed, at full depth (20mm). Depending on your machine, material, and tooling, you could easily go faster with this type of toolpath.

Your toolpath is better than standard roughing, and I have no idea if it would be better than mine. Maybe it is. I only posted it as an example of what you can do with different software, as that seemed to be what you were asking about in your original post. Perhaps I did not understand you clearly, as you seem to already feel that what you have is the best fit for you.
 
hi,
I wanted to thank you compare with other cam software you've been very kind
thanks for the info if I can be of help is a pleasure
I wanted to see some other software what kind of path do thanks again
 
It seems Cax uses 3 trochoid paths to mill out the profile, wich is very uneffiecient, since a trochoid path has alot of air cutting moves, its better to use it only for opening up the slot, then continue side milling ala volumill/truemill or other smart paths that avoid cutting corners with too high tool engagement angle.

dandrummerman21's path is alot more 2012 and will result in faster cycle times and probably longer tool life.

And Cax, dandrummerman21 was actually trying to help you, it doesnt seem he needs education regarding trochoid cutting.
 
I consider much of the advice Xjenderfloip is best used only for the slot opening (Volumill is ok )
The representative gave me the tool parameters and how I had to do the ritch........
I do not have the ability to do otherwise because catia also has a macro opening with trochoid.
for:
thank you very dandrummerman21 do not want to teach anything I just wanted to know if the way I had done could optimize and if there was any software that used the trochoidal well. Taking the path with Catia I with a speed of 1875 rpm and a feed rate of 735 with a milling cutter Ø 16 6 cuts (step diameter trochoidal 1mm) about 14 minutes use single Z-20 mm, also by the way of finishing with a new cutter Ø 16 (with a prehole with a Ø 20).
dandrummerman21 can consider these parameters to your path?
Thanks guys I'll try the short program in CNC machine and will let you know
 








 
Back
Top