Morph Internal Radius Stepover Issues

[Zoffen]

Hey EMC Crew!

 

Is there any way to get Morph between 2 curves to not add so many passes in an internal radius that is close to the cutter dia.

This is using Mastercam 2020

Surface Radius is .260.

Using a .500 Dia Lolipop tool.

As you can see here there are alot more passes  in the internal radius than the rest of the path.

 

This is using "Exact" stepover calculations. However either option will generate the same extra passes on the internal rads.

 

Is there any way to get it to not add all of these passes to the internal radius?

 

 

My guess here is the part of the toolpathing algorithm is trying to calculate an exact stepover on the radius sruface but there is some tolerancing issues with the calculation making it think it needs to add all of those passes to get the desired stepover on the actual internal radius surface. 

 

Thanks in advance!

[crazy^millman]

In a situation like this one break up the toolpath and doing them in section is about the only way I have found to control it like you are asking Combined it is doing what is has been told to do. The tool is given a step over on the surface and on the OD it is meeting that, but on the ID area it is also meeting it if you mapped out the contact point of the tool and measured around the radius you would see yes indeed that step over is exactly what the software was told. Is it insane oh yes and where breaking it up though a pain it does give the programmer exactly the level of control they are looking for.

[Zoffen]

Thanks for the input!

I will probably just live with the extra passes since this is a 1 off.

--

Maybe this might be an area for an enhancement request....

Possibly something like a "Remove/Combine Tight Passes Less Than (Value)" i.e. remove/combine passes where the distance to the next pass is less than the specified distance. Using the max surface step over as the maximum distance for the next pass.

With those two inputs it seems like you could tune the toolpath to get the results for a wide variety of applications.

Hopefully that makes sense to someone!

[Chally72]

19 hours ago, Zoffen said:

Hey EMC Crew!

 

Is there any way to get Morph between 2 curves to not add so many passes in an internal radius that is close to the cutter dia.

This is using Mastercam 2020

Surface Radius is .260.

Using a .500 Dia Lolipop tool.

As you can see here there are alot more passes  in the internal radius than the rest of the path.

 

This is using "Exact" stepover calculations. However either option will generate the same extra passes on the internal rads.

 

Is there any way to get it to not add all of these passes to the internal radius?

 

 

My guess here is the part of the toolpathing algorithm is trying to calculate an exact stepover on the radius sruface but there is some tolerancing issues with the calculation making it think it needs to add all of those passes to get the desired stepover on the actual internal radius surface. 

 

Thanks in advance!

The key thing to remember here is that what you're seeing with the blue lines is the path of the center tip of the lollipop tool- not the actual contact point of the flute against the radius. If you were to draw the actual contact lines for each pass on that radius, you would see a perfectly even stepover. To get rid of these 'extraneous' passes, what we need to calculate by is actually cusp height, not stepover- since in areas where the surface radius gets close to the tool radius, we don't need as many passes to get the same surface finish and we mentally see these close together passes as "wasted" motion. This would mean we'd have to calculate a variable stepover along the surface.

Now, for this example it seems reasonably feasible to do so (calculate a path by dynamic cusp height rather than stepover,) but when you throw in compound surfaces, changing tool axis control at each point along the path, transitioning between radii on the tool with something like an accelerated finishing cutter, etc- it becomes fiendishly difficult to accomplish correctly. We can do this in a path like equal scallop specifically because we've fixed some of these variables- such as we only have one tool orientation.

One old-school way to reduce the pass count would be to offset the surfaces by the radius of your tool, and then generate the path on the offset "centerline" surfaces without tool comp- that way the stepover doesn't contract when projected back to center when it hits the fillet area.

[Zoffen]

Dylan thanks for the explanation. Yes the math and algo's are always more complex than It appears at first.

--

Surface step over based on cusp height producing a variable step over would be a sweet feature. I see how this would be complex to implement tho. Maybe consider it a challenge?

Does any other software have variable step over based on surface cusp height?

 

[Aaron Eberhard]

Hey Zack,

There's a few things going here.  Like Dylan said, it's hard to visualize what the cutter is doing at the contact point instead of what the tip itself is doing.  I find the easiest way to see it (DO NOT POST THIS WAY UNLESS YOU CHANGE YOUR TOOL OFFSET ON THE MACHINE!) is to change this setting:

To make it even easier to visualize, from the side view I drew some .500" circles at the end of the toolpath and then created a point at the intersection of the fillet & cutter ball)

Note for anyone watching at home, I used to save the toolpath geometry) to a level, then deleted the linking moves with QuickMask Colors (on the right side).

So the actual contact patch is not bad.

 But, if you want to get around it, you can do like Dylan said and offset the surface, or, if you're on 2022 you can use Unified Multiaxis in "Guide" mode.  

Same geometry but note the "Style" is set to guide:

And what's making this one better is under Machining Geometries - Advanced parameters:

Which (in a nutshell) will do exactly what Dylan said, it'll just do it for you:

[#Rekd™]

6 minutes ago, Aaron Eberhard said:

(DO NOT POST THIS WAY UNLESS YOU CHANGE YOUR TOOL OFFSET ON THE MACHINE!)

Love the warning!!! Sounds like something that would easily be overlooked!

+1 @Vector Manufacturing!!!!

[Chally72]

26 minutes ago, Aaron Eberhard said:

Hey Zack,

There's a few things going here.  Like Dylan said, it's hard to visualize what the cutter is doing at the contact point instead of what the tip itself is doing.  I find the easiest way to see it (DO NOT POST THIS WAY UNLESS YOU CHANGE YOUR TOOL OFFSET ON THE MACHINE!) is to change this setting:

To make it even easier to visualize, from the side view I drew some .500" circles at the end of the toolpath and then created a point at the intersection of the fillet & cutter ball)

Note for anyone watching at home, I used to save the toolpath geometry) to a level, then deleted the linking moves with QuickMask Colors (on the right side).

So the actual contact patch is not bad.

 But, if you want to get around it, you can do like Dylan said and offset the surface, or, if you're on 2022 you can use Unified Multiaxis in "Guide" mode.  

Same geometry but note the "Style" is set to guide:

And what's making this one better is under Machining Geometries - Advanced parameters:

Which (in a nutshell) will do exactly what Dylan said, it'll just do it for you:

What a helpful anonymous Mastercam multiaxis user. 

 

Thanks Aaron!

[crazy^millman]

Well I learned something so thank you both for the great explanations.

25 minutes ago, #Rekd™ said:

Love the warning!!! Sounds like something that would easily be overlooked!

+1 @Vector Manufacturing!!!!

Problem is people who want to come back and hold you or your company responsible for not thinking to do it.

[Aaron Eberhard]

36 minutes ago, #Rekd™ said:

Love the warning!!! Sounds like something that would easily be overlooked!

+1 @Vector Manufacturing!!!!

That's the warning of experience talking

Thanks!

[Aaron Eberhard]

28 minutes ago, Chally72 said:

What a helpful anonymous Mastercam multiaxis user. 

 

Thanks Aaron!

I'm just a simple passer-by... 

If you flip that switch from Tool Center Mode to Contact Mode, you'll get the same exact results as you would with a Morph set to "Exact."    I probably should have deprecated that before I left.   Ah well, leave that for the poor new guy to deal with

A few other notes on "Tool Center Mode:"  It only works with round tools (Ball, Lollipop), so if you have to use a Bull Nose or some other shape, you'll need to deal with Contact Mode.  If I recall, I covered that some in the "How to leverage Geodesic (Automatic & Guide) options on your parts and some settings that can help you" video that's linked on the Mastercam forum for 2022.

[Zoffen]

Awesome. Just awesome. I love this forum. Thank you for all that gave input.

--

I am not on 2022 yet but will be moving over soon. The unified multiaxis path and options look great.

[lowcountrycamo]

I see this alot where pencil cutter is .120r and fillet is .125r.  In that case I have created surfaces that come to a sharp point and let the tool create the fillet. 

steve austin

[Colin Gilchrist]

2 hours ago, lowcountrycamo said:

I see this alot where pencil cutter is .120r and fillet is .125r.  In that case I have created surfaces that come to a sharp point and let the tool create the fillet. 

steve austin

Yes, if the customer provides a Solid Model, I will often make a copy, remove the history, and then use the "Modify Feature > Remove", to simply delete the fillet faces. The trick here, is to be able to identify the "last operation" which was done on the solid, and "remove those features in reverse order".