feed rates om contors with arcs

[veritasproject]

is there any way in x3 to change the feed in arcs based on its radius. now i have to do it by hand to get the right feedrate on a contor with a radius in it.

[Hardmill]

Why do you need to have different

feed on arcs ??

Calulate a chip for that tool and

material and let er rip.

 

Ive never undestood this concept

of needing different feed rates.

 

I do understand there are some

cases where it is neccessary.

 

 

PEACE

[veritasproject]

If i do that the tool will chater on the inside of an arc on a contour. high finish is what i do this for. On inside arc you need to slow down the feed to hold the same chip load and sfm that you do on a strate line.

[strabe]

"Change at point" is the only way I know of. I don't think you can adjust it based on the radius.

 

HTH

[ATG]

Cant you use Highfeed to get somthing close to what you need......

[veritasproject]

where is the "channge at point option"?

[spade117]

You can set all arcs to one seperate feedrate, but not based upon the size of arc.

[JDowe]

If you go to tool settings there is a box to

adjust feed on arc move - I think it scales

the feed rate based on how close the arc radius

is to the tool radius

[spade117]

quote:

---

If you go to tool settings there is a box to

adjust feed on arc move - I think it scales

the feed rate based on how close the arc radius

is to the tool radius

---

That is what I was talking about...it lets you set a seperate feedrate for arcs, but it's not based upon any scale.

[veritasproject]

you would think that mastercam would scale it right the formula is not that complex

its,

part radius - tool radius/part part radius=a

a x original feed rate= the feed rate for the radius.

 

i just hate having to edit the g code

every time i a good finish

[generaldisarray]

Does anyone else do this?

[RObert TImby]

There is a place in the properties/tool setting lower left that you toggle on and put the feed rate but never did needed to do it. hope it works for you. There is also the toolpath editor thin there also you can change the feed rates as needed for you to post.

[Matthew Hajicek - Singularity]

I use highfeed once in a blue moon. Some posts have change feed on arcs built in too. If you want more control over it you could write your own post section and have it reference misc vars.

[veritasproject]

the tool path editor works thank you but it would be nice if mcx would do it for you

[allena]

I have the same request,I have used other programs that adjust the feedrate with the above formula. It is very useful on older machines that don't have G107 option. I normally use the change at point (in geometry) I recall a post a while back that someone modified their post too use this formula on arcs.I dont like the adjust arcs feed (tool setting page)because it does it for the whole program (slows down roughin ops)I wish it was in each operation.

[Rob @ Target Machine]

This is what I'm using in my post:

 

code:

---

#       mr5$ "Arc Feedrate Factor"  <------------------------multiplies feed by this value

# mr6$ "Arc Threshold" <------------------------------if arc rad falls below this value

 

 

 

 

pcirout1 #Output to NC of circular interpolation

pcan1, pbld, n$, `sgfeed, sgplane, sgcode, sgabsinc, pccdia,

pxout, pyout, pzout, pcout, parc,

[

if arcrad$,

[if arcrad$ <mr6$ & arcrad$ >-mr6$ & mr5$<>0,feed = feed*mr5$]

],

if feed <0.01,feed = 0.01

feed, strcantext, scoolant, e$

---

At least I can have some control "per operation".

 

It's working fine for me. I mainly use it to overcome servo lag and/or tool deflection in small corner radii.

[GIZMO 21]

i use the adjust feed on arc move all the time just for the finishing tool path.when i generate a rough tool path i just go back into the tool setting and uncheck it before i even start the chaining seq.it is very helpful when your running fin. tools @ 120 ipm on straight cuts and you come on inside rad or outside rad. at that feedrate you won't get true rads. because of tool deflection

[GIZMO 21]

i can't believe it took me this long to post something.

[Dowty123]

I don't need to reduce my feeds in corners since I am always (except in very specific cases) taking a tool at least 10-15% smaller then my corner rad. When the roughing has the same amount of stock everywhere (even in corners) and the tool really interpolates, no need to reduce feed in corners. Except if the machine isn't accurate enough or does not have any look ahead option.

 

Simon

[Guest CNC Apps Guy 1]

The big problems come when you use a tool with a radius too close to the corner radius so yes, in those cases you need to adjust the feedrate. The easy way to deal this is to use smaller tools for the finish, then you can run regular feeds and not have to worry about it. For whatever (no good)reason every engineer likes to have .125, .250, .375, and .500 inside radii.

 

I use to like to spec metric tools for finishing (4mm, 6mm, 8,mm, 10mm, and 12mm) used to xxxx guys off but... using a 12mm instead of a 1/2" worked WAY better on finish passes.

 

Sometimes you just gotta think outside the box.

[Matthew Hajicek - Singularity]

You could just spec a 27/64" EM...

[Guest CNC Apps Guy 1]

Isn't a 27/64 a tad bit difficult to find in a Solid Carbide E/M?