Ramp Plunge Moves - Clarification

Discussion/questions about software used with your CNC Shark and programming issues

Moderators: al wolford, sbk, Bob, Kayvon

Post Reply
User avatar
NewAgent45
Posts: 230
Joined: Sun Sep 08, 2013 8:29 am
Location: Edgewater, Florida, USA

Ramp Plunge Moves - Clarification

Post by NewAgent45 »

Please confirm how the ramp plunge moves setting works. As I understand if this function is selected and a ramp distance is entered the tool will cut and angle. For example if I'm cutting a circular vector (hole} 2" diameter inside/left all the way through 1/2 thick material with a ramp distance of 0.375 the starting cut will begin 0.375 inside the two inch vector and end at 2" and the hole. The purpose of this is to reduce spindle load and reduce heat build-up.

Is this right?

Have a great day!
... Rod

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Ramp Plunge Moves - Clarification

Post by Rando »

NewAgent45 wrote:Please confirm how the ramp plunge moves setting works. As I understand if this function is selected and a ramp distance is entered the tool will cut and angle. For example if I'm cutting a circular vector (hole} 2" diameter inside/left all the way through 1/2 thick material with a ramp distance of 0.375 the starting cut will begin 0.375 inside the two inch vector and end at 2" and the hole. The purpose of this is to reduce spindle load and reduce heat build-up.

Is this right?
... Rod
Yes, most end-mill do not like plunging straight down into the material. The ramp length should be at least twice the bit diameter. If you set a longer ramp length, it should double-back on itself, folding the ramp so it goes back and forth as it enters the material. Note that using a ramp, especially on the Sharks, does NOT usually mean that you can then proceed to cut the entire 1/2" hole in one pass. The cut depth needs to be set based on what the material, the bit, and the machine can handle. So, if you're cutting a hole 1/2" deep, and the depth-of-cut is really only 0.1", then you're going to end up with five cuts (six since you'll probably cut a little below the bottom to make sure it's really cut through), and the bit will be ramped down into each cut layer as it goes down.

One of the pain points I've always had with the Vectric software is that it doesn't let me set the "safe height" for those ramps. So, when it's done with one cut-"layer", it goes back up to whatever safe-height it decided on, and then cut air all the way down until it touches the material. That air-cutting can amount to a lot of wasted time. Sorry to say, I don't have a solution to that.

Also, I believe that when it's doing the ramp, it uses the "plunge rate" as the horizontal speed. Normally plunge rate refers to the VERTICAL speed, which would result in a horizontal speed faster than the plunge rate, if done properly. Instead, if you specify a low plunge rate for the tool on that cut, you'll end up with a really long ramp time that is often way slower than necessary.

Hope that provides some guidance.

Regards,

Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

User avatar
bill z
Posts: 342
Joined: Fri Sep 25, 2015 9:09 am
Location: Spring, Texas USA

Re: Ramp Plunge Moves - Clarification

Post by bill z »

I’m new to a bunch of this but I did learn something about ramp distance and plunge rate recently when thinking I could drill holes with my end mill.

Yes, My Aspire software has a drill option but I found that the software expects the correct tool size to drill the hole. Because my projects had 6 different hole sizes, I didn’t want to keep changing bits. So, I figured, I would have the machine make the holes the correct size by cutting inside the circle with a smaller end mill. Problem was the ramp made the hole oblong and not round.

I guess the way around this is to have several tool descriptions for the same end mill, each with different settings.

I would like to know what works best.

User avatar
NewAgent45
Posts: 230
Joined: Sun Sep 08, 2013 8:29 am
Location: Edgewater, Florida, USA

Re: Ramp Plunge Moves - Clarification

Post by NewAgent45 »

Bill,

I'm using V-Carve Pro but I'm pretty sure you have similar options in Aspire.

I only us the Drill toolpath for several holes of the same size.
I often drill holes of various sizes by two methods:

If they are a lot bigger than the bit size I use a profile toolpath. If you select [Select advanced toolpath options] You have the option of Separate last path. This allows you to enter an allowance offset value. I enter a value of a few thousands (like 0.002 - 0.010). Then will cut this amount on the last pass to give a clean edge. I also add tabs if the hole is fairly large.

It the holes you want to drill are relatively small select a bit smaller than the largest hole and select a pocket toolpath. With the pocket tool path you can enter a Pocket Allowance value which works similar to the offset allowance in the profile toolpath.

By the way I have created slotted holes the same way as above by just drawing the vectors as slots.

At any rate I'm not sure your use of the ramp plunge messed up your holes. Perhaps you created a high tool deflection issue do to high loading or the material may have slipped.

Hope this helps!

Have a great day... Rod

Post Reply