Trying to cut just inside this Y shape. Cutter will enter single opening and just cut as far down as possible
I'm having a hard time generating a toolpath for cutting only inside a mesh shape. This will be for 4 axis cutting.
I have my spindle orientation down and have even made some successful cuts... but I can't get a toolpath to cut everywhere that I want it too.
It's for cutting the inside of a cylinder head port.
Which toolpath icon should I be using?
Similar Threads:
Trying to cut just inside this Y shape. Cutter will enter single opening and just cut as far down as possible
You will need to do both holes separately and you will need to align the center of each hole in rhthrough X then make a line in X then choose the line in the pop up window that allows you to choose the axis for the 4th.
If you go to YouTube and type in madcam there is a video
But just looking at the part I do not see how spinning the part on your 4th is going to get you any deeper or more accurate than just stationary mounting it upward on the bed and 3 axis milling . This is really a job for 5 axis
Im not worried about 2 smaller holes. the single hole in 4axis allows cutter to reach in deeper and cut as much as possible by turning part to optimize cutter.
there is more to this drawing, but im trying to concentrate on this part for now. if you go on instagram i have a video up @camdesigner .
i think i have to keep my axis the way they are for how part is being rotated and cut. in video i used curve milling from boundary curve. but it only hits part of model and misses quite a bit. i just cant find correct protocal for which toolpath to use.
hard to see, but this is a screenshot of toolpath. thats all i can get it to cut. ive just tried rotating model, moved spindle drive location.... will only cut in same spot. driving me crazy!
You might want to try down loading the trial version of madcam 5x and using drive surface .
This allows you to create a surface above the part tilt that surface in the same plane that the 4axis tilts and then tool path it will cut everything in the path of the shadow that the drive surface plane sees to the chosen depth you can even chose an angle outside 90 degrees to the surface .
I use 5x all the time with 4 axis set ups as it saves huge amounts of time in head scratching . After trying it once I am sure you will see it is worth the upgrade price
If you need I can shoot a screen shot of what I am referring to .
A screen shot would be great! Thank you
Double post
Make a drive surface ,as in first pic then angle it so you can get around corner , then choose depth set minimum angle to 0 and max angle to 180 then choose , then under simultaneous 5 axis milling button choose roughing , z level or planar,
If it does not make sense let me know.
Sorry pics are upside down . iPad issues , and in the opposite order
Even though I'm only cutting 4 axis I should still choose 5 axis?
If you want to use the drive surface , yes, I use it because it takes away almost all the thinking.
Just don't change madcam machine setup from what you already have
Though in your application you will have reach issues and crash potential as you are milling deep inside a part .
you can also make a curved drive surface to go around an object .
Or choose the surface it self if it only curves in the axis directions have it set up for .
So the toolpath in Madcam doesn't know if cutting bit will crash into sides of model? That's my job to figure out?
yes and no on the crash
mad cam knows when the cutter will touch based on the size of shank you inputed , but above that is the holder and it does not know about that for purposes of pathing . You can model your spindle and holder and input it into madcam for which i still need to do , and I actually need yoakim to do a video or an instruction post . then you can see the whole unit in the simulator to see If there are crashes , but as far as i know madcam sim does not warn you of a crash potential.
because you are going quite deep at a large angle there may be a chance of the holder/spindle crash
some of the others who know this program better than me may also have better advice for you .
Depending on how deep into that port you intend to go, madCAM might not be the best tool for this job. Once you get so far in that holder collisions are an issue, or even holder proximities, then you might have problems as Gregore mentioned. We use WorkNC for complex 5-axis simultaneous cutting because it has full holder collision protection (and can even automatically tip the tool to avoid the shank or holder from rubbing or colliding).
I know this isn't overly helpful, but you do need to be aware of the limitations. Of course, it's possible that there are 5-axis features I'm unaware of because we use WorkNC for this type of work, so I would be happy to be corrected (and learn something at the same time!)
Dan
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
one thing I have done is load that section of the gcode and run just the area I am worried about at really slow speeds to see . you could also lie a little to nadcaym about the diameter of the shank of the cutter ( make it bigger and longer than it is) so madcam gives you extra clearance .