flowline stepover

[danatoem]

I have often noticed that when using flowline and specifying a step over, say of .002  that it will increase dramatically around a radius. I am machining a tapered wall (up and down motion in the Z axis) that wraps into a radius just now and wonder if there is a way to get a consistent stepover thru both?

[AHarrison1]

Use Scallop height instead of Distance.

 

[danatoem]

I noticed when using scallop that it REALLLLLLLY  tightens up around the radius!  and then makes  more of a step in the flat wall.  Think i will stick with scallop! 

Thanks

 

[AMCNitro]

Try cutting in the other direction.  Why are you cutting up and down?  Instead of left to right?

[danatoem]

Because i need a sharp corner at the bottom and i am using a sharp end mill

[Jake L]

23 hours ago, AHarrison1 said:

Use Scallop height instead of Distance.

 

Wanted to do an in depth explanation of this because it took me a long time to figure out when to use stepover vs scallop and why.

Tool center and tool contact point are two different things. The toolpath lines we see in backplot are where the center of the tool will be.

When surfacing around a radius and driving by stepover, the center of the tool must take larger steps to keep the stepover at the contact point consistent. 

In these pictures you can see when driving the toolpath based on the stepover, the stepover around the radius stays consistent at .099-.100, but the tool center stepover is much larger around .298. 

An unexpected consequence of using stepover is the scallops around a radius will be bigger or smaller than scallops left on flat surface.

When using scallop to drive the toolpath, you tell Mastercam you care more about the height of the scallop than the stepover. This causes the stepover of the contact point to shrink around outside radii and grow around inside radii.

Dropbox Link To File and Pictures (MC2023)

Please correct me if there are any mistakes in this explanation. I think I have a solid understanding of this concept but there's always more to learn. Hope this helps!

[AHarrison1]

19 minutes ago, Jake L said:

Wanted to do an in depth explanation of this because it took me a long time to figure out when to use stepover vs scallop and why.

Tool center and tool contact point are two different things. The toolpath lines we see in backplot are where the center of the tool will be.

When surfacing around a radius and driving by stepover, the center of the tool must take larger steps to keep the stepover at the contact point consistent. 

In these pictures you can see when driving the toolpath based on the stepover, the stepover around the radius stays consistent at .099-.100, but the tool center stepover is much larger around .298. 

An unexpected consequence of using stepover is the scallops around a radius will be bigger or smaller than scallops left on flat surface.

When using scallop to drive the toolpath, you tell Mastercam you care more about the height of the scallop than the stepover. This causes the stepover of the contact point to shrink around outside radii and grow around inside radii.

Dropbox Link To File and Pictures (MC2023)

Please correct me if there are any mistakes in this explanation. I think I have a solid understanding of this concept but there's always more to learn. Hope this helps!

This is exactly how I understand it to work hence my suggestion.

Thank you for the detailed explanation.

If it is wrong then both you and I stand corrected.

[KMartin]

Thanks for the info guys .Great explanation .  

[AMCNitro]

On 10/30/2023 at 11:12 AM, danatoem said:

Because i need a sharp corner at the bottom and i am using a sharp end mill

It will still work...

[SuperHoneyBadger]

33 minutes ago, AMCNitro said:

It will still work...

I was thinking the same thing when I read this thread a few days ago. The last pass will run along the bottom of the wall and leave a sharp edge. We do it all the time.

[danatoem]

Just to respond to the question why not go left to right, or across the face as opposed to up and down? When you go across wall that has draft on it, with a sharp endmill the result will be a finish that will resemble a stair case. When using a sharp endmill on a drafted wall and going up and down the finish will  be smooth as a babies butt! You will be using the radius of your endmill as opposed to a sharp corner . It also just happens that this drafted wall had a sharp corner at the bottom or i would have used a bull mill or , say a 1/8 e/m with .03 corner rad. The easy thing would of been to use a taper cutter but this wall has odd ball draft. 

[AMCNitro]

On 11/2/2023 at 1:33 PM, danatoem said:

Just to respond to the question why not go left to right, or across the face as opposed to up and down? When you go across wall that has draft on it, with a sharp endmill the result will be a finish that will resemble a stair case. When using a sharp endmill on a drafted wall and going up and down the finish will  be smooth as a babies butt! You will be using the radius of your endmill as opposed to a sharp corner . It also just happens that this drafted wall had a sharp corner at the bottom or i would have used a bull mill or , say a 1/8 e/m with .03 corner rad. The easy thing would of been to use a taper cutter but this wall has odd ball draft. 

Depends what you step down is.  I use it all the time making molds, I rarely use taper endmills anymore.  I also use Countour with an angle A LOT.  2 or 3 degrees with a .004 step downs leaves a pretty nice finish.

[Newbeeee™]

On 11/2/2023 at 9:33 PM, danatoem said:

Just to respond to the question why not go left to right, or across the face as opposed to up and down? When you go across wall that has draft on it, with a sharp endmill the result will be a finish that will resemble a stair case. When using a sharp endmill on a drafted wall and going up and down the finish will  be smooth as a babies butt! You will be using the radius of your endmill as opposed to a sharp corner . It also just happens that this drafted wall had a sharp corner at the bottom or i would have used a bull mill or , say a 1/8 e/m with .03 corner rad. The easy thing would of been to use a taper cutter but this wall has odd ball draft. 

I would also use the "up and down" as often as possible - on average (neck out) you get a better finish for a lot less toolpath travel (= less cycle time)

@Jake L nice explanation

[Kyle F]

5 hours ago, Newbeeee™ said:

I would also use the "up and down" as often as possible - on average (neck out) you get a better finish for a lot less toolpath travel (= less cycle time)

@Jake L nice explanation

this is blowing my mind,... so y'all do surface finishing, with square endmills, feeding up and down?!

Is this only on tapered surfaces, or vertical walls as well? I could be misunderstanding, but this is very intriguing to me.

[SuperHoneyBadger]

2 hours ago, Kyle F said:

this is blowing my mind,... so y'all do surface finishing, with square endmills, feeding up and down?!

Then you would love the 45° ruffing I just ran. Cut the time in half for those ops - ran along the wall on 45's and spooked the operator.

And yea, we have some steel parts with 7 or 15° tapered walls about 2.0" tall, and one 45°x.500 chamfer that is the wall of a critical pocket . We run up and down on those too.

[AMCNitro]

2 hours ago, Kyle F said:

this is blowing my mind,... so y'all do surface finishing, with square endmills, feeding up and down?!

Is this only on tapered surfaces, or vertical walls as well? I could be misunderstanding, but this is very intriguing to me.

There's a very common misconception that if it's not straight you have to use ball EMs.  I make small molds now, usually nothing bigger than .25 EM.  But when I made bigger molds with more shapes, I'd rough everything with a square EM, much more efficient that ball.  Ball EMs tend to load up with heavy cuts, so I just take out as much material with a square EM and then go in there and semi finish and finish with a ball, or even a bull if possible.  Even making molds for small parts I first rough it out with square EM, Im talking 1/32 diameter.  MC does all the calculations for you.  

 

[Newbeeee™]

3 hours ago, Kyle F said:

this is blowing my mind,... so y'all do surface finishing, with square endmills, feeding up and down?!

Is this only on tapered surfaces, or vertical walls as well? I could be misunderstanding, but this is very intriguing to me.

Yep where possible - talking predominantly aluminium.

For steels I'd be running a bull mill - say 0.5 (20 thou) corner rad on the tip as a strengthener.

Only talking chamfers or angled walls.

[Kyle F]

On 11/9/2023 at 8:51 AM, SuperHoneyBadger said:

Then you would love the 45° ruffing I just ran. Cut the time in half for those ops - ran along the wall on 45's and spooked the operator.

And yea, we have some steel parts with 7 or 15° tapered walls about 2.0" tall, and one 45°x.500 chamfer that is the wall of a critical pocket . We run up and down on those too.

For some reason it took me years and years of programming to really start to implement ramping. I think when I was first getting started my old clapped out machine would just give terrible finish when moving in x/y/z at the same time. Now about a decade later I'm running much more capable equipment so I'm doing it a lot more now. It really made me a believer. so satisfying to get rid of those lead ins/outs on every depth cut. and I like to rough with bull endmills so I feel like they really enjoy heavy ramp angles. Now I'm going to have to start to change my way of thinking with this whole vertical finishing thing lol! Can't wait to get a part where it makes sense to give it a shot!

 

23 hours ago, AMCNitro said:

There's a very common misconception that if it's not straight you have to use ball EMs.  I make small molds now, usually nothing bigger than .25 EM.  But when I made bigger molds with more shapes, I'd rough everything with a square EM, much more efficient that ball.  Ball EMs tend to load up with heavy cuts, so I just take out as much material with a square EM and then go in there and semi finish and finish with a ball, or even a bull if possible.  Even making molds for small parts I first rough it out with square EM, Im talking 1/32 diameter.  MC does all the calculations for you.  

I definitely agree with you there! Usually the smallest ballmill I'll use is 1/16, and I'll always rough it with a bull or square endmill. I was watching IIRC the mastercam youtube video series "ron week" and ron was talking about ball endmills and how at the very tip, it's cutting at 0sfm. it made me chuckle but I had never thought of it like that and it makes perfect sense. 

 

23 hours ago, Newbeeee™ said:

Yep where possible - talking predominantly aluminium.

For steels I'd be running a bull mill - say 0.5 (20 thou) corner rad on the tip as a strengthener.

Only talking chamfers or angled walls.

understood!

[Jake L]

1 minute ago, Kyle F said:

I'm going to have to start to change my way of thinking with this whole vertical finishing thing lol! Can't wait to get a part where it makes sense to give it a shot!

Agree with you here. I programmed a part earlier this year that this would've working perfectly on. 

[cruzila]

3 hours ago, Kyle F said:

"ron week" and ron was talking about ball endmills and how at the very tip, it's cutting at 0sfm.

Every tool that rotates has 0 SFPM at the center. Endmills are cupped so unless the ramp is greater than the cup size it won't cut to the center. Crazy when you really start to think about it.

Vertical cuts can be good on straight angles. If you make a vertical cut on a radius it will facet it at the tolerance as set. I like to go lefty righty on radius because of this.