Calculating Ramp Angles- Swift Carb Ramp Mill

allloutmx · May 18, 2015

I just purchased a new tool that advertises ramping at 12-17 degrees. http://swiftcarb.com/catalog/SwiftCarb2014.pdf

With that said... If I am ramping down through the material(aluminum), and the perimeter of the path is roughly 24 inches.

Given an angle of 15 degrees, what would my depth per pass be on this path.

My formula looks like this- TAN 15 = X/24

The answer doesn't look right to me... Typically I interpolate at anywhere from .005-.02" depending on material, finish and tolerance desired etc etc. Since this is a new tool, I'd like to push it to its advertised limits without breaking it. Any help would be greatly appreciated.

Joec@westminster · May 18, 2015

are you ramping for the entire perimeter like MC does? or does it ramp to level from the previous level like in NX? Worlds apart in results there. For example, In the scenario you point out, your ramp depth is 5.6254", I agree that seems off.

With NX I specify ramp angle and doc. So if my doc is .1" and my ramp angle is 15* it will ramp for a distance equal to .1/tan15=.3732 and then continue around the part and start the process over till the desired depth is achieved.

With Master Cam, you can spec out a doc or a ramp angle and you will achieve a constant doc all the way to the bottom. As I see it with your new cutter, you need to figure what you want for a doc and then trig out the actual ramp angle if you want to know what the angle is.With MC I always specified the doc and let the software worry about the angle.

Joe

Thomas Paine · May 18, 2015

tan O = z / x
tan 15 = z / 24.
z=6.430
make sure you are degrees and not radians. if the answer yields in the 20's then you are in radians.

allloutmx · May 18, 2015

Thomas Paine said:
tan O = z / x
tan 15 = z / 24.
z=6.430
make sure you are degrees and not radians. if the answer yields in the 20's then you are in radians.

I just needed to make sure I was correct in my figuring. I got the same answer... just like the first time I used a carbide drill, I am a bit shell shocked by the numbers we are getting. I called the MFG... they said yeah let her rip.

Joec@westminster · May 18, 2015

Huh, I must have had something piled on my calculator because I can not duplicate my original answer....I come up with the same answer as Thomas. :cheers:

allloutmx · May 18, 2015

Joec@westminster said:
are you ramping for the entire perimeter like MC does? or does it ramp to level from the previous level like in NX? Worlds apart in results there. For example, In the scenario you point out, your ramp depth is 5.6254", I agree that seems off.

With NX I specify ramp angle and doc. So if my doc is .1" and my ramp angle is 15* it will ramp for a distance equal to .1/tan15=.3732 and then continue around the part and start the process over till the desired depth is achieved.

With Master Cam, you can spec out a doc or a ramp angle and you will achieve a constant doc all the way to the bottom. As I see it with your new cutter, you need to figure what you want for a doc and then trig out the actual ramp angle if you want to know what the angle is.With MC I always specified the doc and let the software worry about the angle.

Joe

Im using Esprit on this project. Its is asking for an incremental spiral depth in distance per rev, not degrees.. I am use to using depth per rev, as that's what Im used to with mastercam, but since Im trying to use the tools capabilities, I want to make sure Im within that envelop of 12-17 degrees of depth per rev.

At .3 total depth of cut, Ill be to depth and full slotting real quick that's for sure. Ill let you fellas know how she cuts!

NAST555 · May 18, 2015

Yeah Z is 6.4 and your calculation is correct but 15 degrees? WOW!! I would like to see if that sucker can hold up to it. That means that the clearance at the back of the flutes is more than 18 degrees and cannot rub at those ramp angles. I get what you are saying that you want to use it as intended but I have learnt the hard way that sometimes the quoted ramping to real life usage may differ. All the best! I hope that it shreds through the material like butter

If it is in a straight line then that is correct but make sure that it is not a radius because then you will have to work out the circumference " 2 x pi x radius)

angelw · May 18, 2015

allloutmx said:
Im using Esprit on this project. Its is asking for an incremental spiral depth in distance per rev, not degrees.. I am use to using depth per rev, as that's what Im used to with mastercam, but since Im trying to use the tools capabilities, I want to make sure Im within that envelop of 12-17 degrees of depth per rev.

At .3 total depth of cut, Ill be to depth and full slotting real quick that's for sure. Ill let you fellas know how she cuts!

Hello allloutmx,
Ramp angle when associated with a helical path equates to the helical angle and therefore the circumference of the helical path and not just the diameter (see attached picture below). Accordingly, the algorithm is as follows:

Z = Tan(helical angle) x Pi x D

Z= Tan(15) x Pi x 24

Z = Tan (15) x 75.3982

Z = 20.2029

Regards,

Bill

RTM · May 18, 2015

Quick clarification here since I see two different answers.

I read the original post to say the "perimeter was roughly 24". Is this the actual length of the path the cutter will take measured at the centerline of the tool or the length of the profile of the part in one complete circuit?

If it is the total length of the XY centerline toolpath, what difference does it make if the move is linear or interpolated as far as calculating the ramp angle? I'm stumbling over this concept.

angelw · May 18, 2015

RTM said:
Quick clarification here since I see two different answers.

I read the original post to say the "perimeter was roughly 24". Is this the actual length of the path the cutter will take measured at the centerline of the tool or the length of the profile of the part in one complete circuit?

If it is the total length of the XY centerline toolpath, what difference does it make if the move is linear or interpolated as far as calculating the ramp angle? I'm stumbling over this concept.

Indeed. I missed the perimeter; in that case it would simply be Z = Tan(15) x 24. However, its rare that you know the perimeter (circumference, if the path is circular) ahead of executing the calculation for Z. Accordingly, the algorithm is still Z = Tan(helical angle) x Pi x D. Most CAM software will use the Diameter or Radius of a feature and not prompt for the circumferential distance when calculating a Helical path.

Regards,

Bill

RTM · May 18, 2015

angelw said:
Indeed. I missed the perimeter; in that case it would simply be Z = Tan(15) x 24. However, its rare that you know the perimeter (circumference, if the path is circular) ahead of executing the calculation for Z. Accordingly, the algorithm is still Z = Tan(helical angle) x Pi x D. Most CAM software will use the Diameter or Radius of a feature and not prompt for the circumferential distance when calculating a Helical path.

Regards,

Bill

I have read too many of your posts to think you made a mistake

I figured you missed the perimeter reference. That's why I wanted to clarify. But I still have a question you may be able to answer.

My other question is still open. Is the correct calculation based off of the centerline of the toolpath or the profile edge or does it make no difference? I have had instances where I have ramped into a part well within the limits of my tool and with parameters based on previous tool usage but yet sometimes the tool sounds a little rough on "weird" profiles (non circular).

I have assumed that the ramp angle calculations should be calculated from the centerline of the toolpath and it makes no difference whether the path is circular or linear. I believe this to be correct but yet somehow I believe there must be a finer calculation that must be done based on the cutter diameter, especially when ramping inside corners. Am I crazy? Has anyone else observed this behavior on larger diameter endmills? Anything I'm not considering here?

And sorry to OP if this is a hijack. This seemed to be the right thread to ask.

EDIT: I said that some tools sounded rough on "non-circular" toolpath and "inside corners" which is not quite right. What I meant to say is that I'm not talking the special case of a helix but an irregular toolpath that contains both linear and arc moves, usually in a pocket where the radial engagement can be up to 100%. I don't know if this clarifies my question or not, I just know that I have my ramping mostly down pat but there are moments when I get surprises with larger tools. Knocking out a slug from the center of a part might present the best visual but I don't mean that particular special case either. Possibly the % width of cut comes into play here?

allloutmx · May 18, 2015

RTM said:
My other question is still open. Is the correct calculation based off of the centerline of the toolpath or the profile edge or does it make no difference? I have had instances where I have ramped into a part well within the limits of my tool and with parameters based on previous tool usage but yet sometimes the tool sounds a little rough on "weird" profiles (non circular).

I came up with 24" as the outside perimeter of the feature, not centerline of the tool path. The shape being cut is a rectangle. My calculation is based on finding my Z depth after making one complete revolution of the 24" perimeter. With any given angle we can find our total Z depth per revolution.

When you say it sounds wierd.... like crunchy wierd? Most the times I have found if ramping to steep, the chips will not clear and I end up recutting chips... which(in steel) sounds like you have rocks in the hole while you are cutting.

Click to expand...

RTM · May 18, 2015

Crunchy is probably an excellent description of the sound, weird is what I would define as the toolpath. Ramping along just fine full width (or again, even partial width) and then the toolpath enters some complicated geometry and it looks by eye to be a plunge just a little too steep but the math is there. I have experienced this in steels as well as harder plastics.

In the example of your rectangle, is your toolpath rounding the corners or making a 90?

TCEDM · May 18, 2015

It's should just z ramp to the depth your telling it to go to.So if your going .5 deep on a pass it will ramp to the .5 deep.If your wanting to pocket the rectangle out.It should start in center ramp down to depth then spiral out rest of material.Then go back to zero and ramp to next depth.I would not want to travel 24 inches and ramp the full length of 24 inches.Ifwe are talking same thing

allloutmx · May 19, 2015

RTM said:
In the example of your rectangle, is your toolpath rounding the corners or making a 90?

Cant show you the entire part but you can see the two profiles I am ramping down. Successfully ramping at 10 degrees, 9000rpm at 70ipm... 15% spindle load. cant even hear the cut. definitely can afford to step it up but im going to ease my way into that confidence.

dstryr · May 19, 2015

allloutmx said:
View attachment 139844

Cant show you the entire part but you can see the two profiles I am ramping down. Successfully ramping at 10 degrees, 9000rpm at 70ipm... 15% spindle load. cant even hear the cut. definitely can afford to step it up but im going to ease my way into that confidence.

I would increase the feed before I increased the ramp angle.

allloutmx · May 19, 2015

dstryr said:
I would increase the feed before I increased the ramp angle.

pretty much what I was thinking. First part just came off the CMM and I don't appear to have induced and more stress into the part. Took 6.5 minutes off my cycle with this tool alone... close to 25 minutes less than the quoted time per piece.

Captdave · May 19, 2015

We use Alumingators from GW Schultz (basically the same tool could be a re brand) to rough out deep counter bores in 6061 T6 at 15* ramp 12,000 RPM 200 IPM down to 1.25" deep x 1.25 Dia. They claim 27* max ramp for pocketing but never tried, a guess would be less then 10 seconds per hole anyways and sounds really sweet.

Calculating Ramp Angles- Swift Carb Ramp Mill

Titanium

Aluminum

Hot Rolled

Titanium

Aluminum

Titanium

Stainless

Diamond

Cast Iron

Diamond

Cast Iron

Titanium

Cast Iron

Aluminum

Titanium

Diamond

Titanium

Titanium

Similar threads