Can we talk about 3D Blend for a minute?

[nperry]

Z2G included. 

Could I find a different way to do that top chamfer? Yes. Do I want to? No. Seems like a perfect opportunity for a really nice blend path.

Maybe someone can look at that and tell me what I'm missing on that path. For whatever reason it won't drop down past a certain depth and I think it's geometry related. In the past I've had to manipulate the geometry to get the path to work nicely, but I figured the addition of "Tool Contact Point" on boundaries would remedy the geometry manipulation issue. Having to do that is tedious and a time suck, so I've largely avoided blend in the past for that reason. 

I feel like I remember reading somewhere on this forum that someone had largely replaced their use of flowline with blend because it was producing finer results. Wouldn't mind seeing some examples of how others are using blend to expand my use of the path a little bit if anyone is willing to play along.

MYSTERY PART.ZIP

[gcode]

I could not find an mcam file in that download

[nperry]

Users -> tgolden -> desktop....

Maybe?

[gcode]

found it

Blend is driven by the C/L of the tool

I just used the command offset/chain and offset the inside chain .06, turned off depth limits and got a pretty nice toolpath

 

 

[nperry]

35 minutes ago, gcode said:

found it

Blend is driven by the C/L of the tool

I just used the command offset/chain and offset the inside chain .06, turned off depth limits and got a pretty nice toolpath

 

 

This is exactly what I would've done in the past. I just feel like I'm missing something. Functionality was added to control from contact point, but it doesn't quite work as expected? Or is it just me?

[TheePres]

Blend was a goto toolpath for me until i discovered morph between 2 curves. It works very similar and you can lock at 3 axis if needed. 

[gcode]

16 minutes ago, TheePres said:

Blend was a goto toolpath for me until i discovered morph between 2 curves. It works very similar and you can lock at 3 axis if needed. 

these are amazing toolpaths, but they create point to point code

this is not important when you have a modern machine tool with adequate memory

but if you're feeding  80's or 90's vintage machines with 125k of memory morph is not an option

 

[Tim Johnson]

29 minutes ago, gcode said:

these are amazing toolpaths, but they create point to point code

this is not important when you have a modern machine tool with adequate memory

but if you're feeding  80's or 90's vintage machines with 125k of memory morph is not an option

 

Back somewhere in the early to mid-nineties another programmer and I went to the Whirlpool model shop to look at their BTR system. What they did for their dinosaurs back then was strap 80 meg hard drives (largest on the market at that time) and ran their programs from there with the BTRs between the hard drives and machines. It was a nice setup. Also, every person in that shop including the machinists was in dress clothes and wearing ties. We had that info in advance so I dressed up with a tie and the other programmer was dressed up but without a tie. The machinists would talk to the both of us but the supervisor would only talk to me. I thought that was rather rude but we were told how they would be dressed.

[Colin Gilchrist]

1 hour ago, gcode said:

these are amazing toolpaths, but they create point to point code

this is not important when you have a modern machine tool with adequate memory

but if you're feeding  80's or 90's vintage machines with 125k of memory morph is not an option

 

This can be overcome if necessary, but its probably more work than is worth the effort. But sometimes Morph just gives you that "clean path", so it is worth the extra effort to filter the path.

> Create the Morph path "as you normally would", but be sure to use a Spiral cut pattern.

> Backplot the path and save as Geometry to a level.

> Clean up path by removing entry/exit and retract moves.

> Create a Contour Toolpath. Chain the spiral motion. Disable "infinite look ahead".

> Set path to "Off" for compensation. 

> Adjust Line/Arc filter as necessary. (You won't get Arcs with spiral motion.)

> After the path has generated, run the Arc3D Chook.

> You'll end up with a pretty clean path, and minimal NC Code.

I took a 400 Kb Morph path, and the resulting Contour was 143 Kb.

After running Arc3D, the result was a path ar 57 Kb. Not bad...

Still, it is a lot of extra work...

[crazy^millman]

Can I ask a dumb question here?

It is a 5 Axis machine why not swarf that chamfer and call it a day?

 

[crazy^millman]

I took OP3 and reprogrammed it with tilt lines for the only wireframe and did everything you were doing in 9 operations. Let me know what you think. I did the walls with 2 methods to show you how to do what your were doing with wireframe without needing to draw the wireframe and still get what your were after. 

Really confused by the OP3 WCS X Axis not matching the OP3 Index operations X Axis. Why are they 90 degrees to each other? I normally make all of them align to each other, but if it works for you then okay, but through me off a little bit.

I named your operation groups. I also renamed the operations in the those groups so when you post them they all don't post out with the same name. I also added viewsheets to the file to show you how I like to use them to help me communicate setup and other things to customers when I send them files I have programmed for them. Hopefully this is helpful and gives you some idea things you can do with Mastercam.

Have a good weekend.

Link to the file. 5TH AXIS MYSTERY PART OP3

[Leon82]

On modern machines sometimes I feel that the paths work smoother with no arcs with lookahead set to roughing.

[SlaveCam]

I have tried making external fillet with blend but it never goes down to the lower chain, for some reason, whatever I try, "Tool contact point" is never un-grayed

[JParis]

Blend works on the driving chains on the centerline...

The inner curves, I always offset by .001" less that half the dia of the tool...that keeps it from diving down further

[Maclaw]

On 10/12/2022 at 1:43 PM, SlaveCam said:

I have tried making external fillet with blend but it never goes down to the lower chain, for some reason, whatever I try, "Tool contact point" is never un-grayed

You have to have projection set to 3D instead of 2D on the Cut parameters page. Then You can use tool contact point with the curves (dont confuse it with the boundry). I dont know why this is so, but that's the way it works. I struggled with it for a while also... But You propably know this by now - I'm a year late sorry

[jpatry]

On 8/13/2021 at 2:41 PM, gcode said:

amazing toolpaths, but they create point to point code

Yeah, and I understand why arc filtering is impossible.

But having some sort of way to reduce gcode size would be nice, would probably require a spline interpolation mode on the machine though.

[JB7280]

On 8/13/2021 at 5:56 PM, crazy^millman said:

I took OP3 and reprogrammed it with tilt lines for the only wireframe and did everything you were doing in 9 operations. Let me know what you think. I did the walls with 2 methods to show you how to do what your were doing with wireframe without needing to draw the wireframe and still get what your were after. 

Really confused by the OP3 WCS X Axis not matching the OP3 Index operations X Axis. Why are they 90 degrees to each other? I normally make all of them align to each other, but if it works for you then okay, but through me off a little bit.

I named your operation groups. I also renamed the operations in the those groups so when you post them they all don't post out with the same name. I also added viewsheets to the file to show you how I like to use them to help me communicate setup and other things to customers when I send them files I have programmed for them. Hopefully this is helpful and gives you some idea things you can do with Mastercam.

Have a good weekend.

Link to the file. 5TH AXIS MYSTERY PART OP3

Hey Ron, I was checking out your file, and had a couple questions.  When you machined the floors in the pockets, you used a Horizontal toolpath.  Any particular reason you use that, versus area mill, or pocket?  Just different ways to skin the cat?  Or is horizontal better in some way?

 

Also, when stepping down the pocket like you are, in the swarf and Surface Contour toolpaths, I almost always end up with steps, or ridges on the walls.  What's your trick to eliminate that??

 

Oops....I also just noticed the date on that post 

[crazy^millman]

3 hours ago, JB7280 said:

Hey Ron, I was checking out your file, and had a couple questions.  When you machined the floors in the pockets, you used a Horizontal toolpath.  Any particular reason you use that, versus area mill, or pocket?  Just different ways to skin the cat?  Or is horizontal better in some way?

 

Also, when stepping down the pocket like you are, in the swarf and Surface Contour toolpaths, I almost always end up with steps, or ridges on the walls.  What's your trick to eliminate that??

 

Oops....I also just noticed the date on that post 

Different way to skin the cat is correct.

Without a real world example no where to know why you are getting steps or ridges. If the shape cannot really be swarf cut and should be surface machined then that would by one reason why that would happen.

[nperry]

8 hours ago, JB7280 said:

Hey Ron, I was checking out your file, and had a couple questions.  When you machined the floors in the pockets, you used a Horizontal toolpath.  Any particular reason you use that, versus area mill, or pocket?  Just different ways to skin the cat?  Or is horizontal better in some way?

 

Also, when stepping down the pocket like you are, in the swarf and Surface Contour toolpaths, I almost always end up with steps, or ridges on the walls.  What's your trick to eliminate that??

 

Oops....I also just noticed the date on that post 

This was my file initially. I couldn't use the doctored file because those pockets were tight and I needed cutter comp on them, so no dice on the surface contour or swarf cutter paths walking down those walls.

One trick I use pretty regularly to get rid of steps or help minimize deflection is to add a spring pass into the path, except run it conventional instead of climb. That'll help suck the cutter into the work instead of push it away and it really helps to take out that last stubborn couple thou.