Backplotting point distribution

[sendithard]

The point distribution on this back plot is showing a lot of points for a straight surface. It is a roughing strategy with wall stock left at .005 and tolerance set to .001.  Why would the straight aways contain so many points?

Also, if I use verify instead of back plotting I can see the stock getting removed. My issue is if I want to see a wireframe in this setting, wireframe click box doesn't do anything regardless of whether I have stock or model check marked.  If I'm looking to see the bull end mill radius matching up with a CAD model fillet should I be using wireframe in back plotting mode instead of verify?

 

Thanks.

[Colin Gilchrist]

Fun fact: these paths create point-to-point motion, "by default".

You need to use the Toolpath Filter settings, and also check your Control Definition Settings > to be sure "Helix motion" is enabled.

I'd suggest a Total Tolerance of 0.002. Enable the "Line/Arc Filter". (Do not use Smoothing).

Set your Cut Filter / Line/Arc Filter Ratio, at 50/50. (0.001 Cut Tolerance, and 0.001 Filter Tolerance.)

These values are "Inch values" by the way. Metric would be 0.05 mm Total Tolerance, and 0.025 mm for both Cut Tolerance and Filter Tolerance.

Make sure the checkbox for 'allow helical arc entry' is enabled.

[sendithard]

Colin,

Thanks for the help. That cleaned it up!

 

[Colin Gilchrist]

I don't think your Control Definition is setup correctly. You should be getting "helix" moves for the spiral down to the floor, and you should be getting "helix" moves, on each of the arcs, which connect the passes...

Can you post a Mastercam File in this thread? Strip out the stuff you don't want, but that Control Def looks like it needs to be adjusted. Both the "Arc Settings", and the Tolerances. (There is a setting where "if the helix height is less than a certain distance", it won't create the helix. I set mine to 0.00004" (40 millionths, or smaller), so I can be sure to get actual Helix motion in my NCI data.)

[sendithard]

Colin,

I'm working on finishing this part up today. I've been delaying learning MC and finally broke thru a learning curve and have my arms around it to play on my own.

I'll have this program posted later today, thanks for offering to look.

[sendithard]

I finished the tutorial project. This go around, I wanted to learn more tools so I imported a vice, stock, part as separate step files and put them on separate levels before doing anything else.  Everything seems good. I adjusted what you said earlier to the best of my ability. Attached is the file.

I'm baffled why the opti rough is trying to face off above the part. I already did a facing operation to top of part which is G54. I played with rest machining, but to no avail.

I'm really confused on why you gotta throw in so many stock models...below is a pic showing my steps on how many times I had to define a stock model.

1st pic below is my current point distribution.  Thanks.

 

 

Titan.emcam

[Chally72]

23 hours ago, sendithard said:

I finished the tutorial project. This go around, I wanted to learn more tools so I imported a vice, stock, part as separate step files and put them on separate levels before doing anything else.  Everything seems good. I adjusted what you said earlier to the best of my ability. Attached is the file.

I'm baffled why the opti rough is trying to face off above the part. I already did a facing operation to top of part which is G54. I played with rest machining, but to no avail.

I'm really confused on why you gotta throw in so many stock models...below is a pic showing my steps on how many times I had to define a stock model.

1st pic below is my current point distribution.  Thanks.

 

 

Titan.emcam

Hey Sendithard,

The Titan tutorials do a great job of showing a single process to get a working part file, but they just don't have the time to go into the depth that is offered by the different types of stock models in Mastercam.

Optirough will create a "facing" cut on the top of the part if it still sees stock left to clean. This is to ensure it can safely take its first full stepdown cut. There's a lot of options here that may be the cause, but making sure it correctly knows that you faced the part in the previous op, then correctly setting your stepdown and your Min and Max Z depths for the Opti, are key points that will determine whether it makes your ghost cut or not.

 The Titans tutorial gets around this issue by telling you to make your stock as if you already faced the part. So to follow their flow, you need to lower the face of that stock block that you drew. In your part file, I just used Model Prep Push Pull to drop the top of your stock block on Level 2 by 0.020 to match the top of the part, then regenerated the Optirough, and no more false facing cut!

The "proper" way to handle this on your real parts in the future would be to make another Stock Model as Op 3 that represented the part after you took that facing cut, and then your Optirough would be Op 4 and would use the Op 3 stock as its Starting Stock. This is a little overkill for the Titans lesson, so they left it out for the sake of simplicity.

 

 

Here is a video that might help with explaining the more advanced use cases of those different types of stock:

 

 

[sendithard]

Chally,

Very informative, thanks. I watched that video and a lot clicked.

I'm decent with fusions cam/hsmworks and to avoid the ghost cutting of material that's already been faced or whatnot you just click rest machining and then select 'from previous operation' and it avoids already cut areas.  Here it seems, as you stated, you must create the stock that has been cut. That seemed more work until I saw the power in making stock along the way as you said. Specially for flipping the part. I was going to venture down that road later, I read you can do the old stl route, but this video cleared up the more efficient way.

 

So below you can see I am doing another part and just for fun I'm trying to make a new stock. What has me confused is you can't select multiple operations? So if I wanted to create a new stock before I flip the part, I would need to intelligently make multiple new stocks along the way making sure to pick up on the important cutting operations so when I flip it there won't be extra stock somewhere on the part?  I would think you could just click all the operations and the stock would be what it would look like in the verify simulator.

 

Below is the pic where I can't select multiple operations to create a new stock. I can only select one operation.  Am I seeing this correct?

Thanks.

 

[sendithard]

Alight, I played around and it appears you CAN select multiple operations to create a stock.....I failed to see the green checkmarks, I was expecting each op to get highlighted...below are the green check marks I missed. It's these little issues that drive me absolutely crazy learning new software.

By the way in that video the gentleman timestamped below has done a facing op, then goes straight into optirough without the ghost cutting issue I had. I'm going to dig around and try to clean mine up, but I'm curious how he got around that:   https://youtu.be/aWKRHmsO2PQ?t=1148

 

 

[Chally72]

Glad you got some value out of the video!

To explain how that part I showed in the video gets around the ghost cut:

If you turn on your Minimum Z height in the Steep/Shallow parameters, and it is greater than the height of the stock that you're telling the operation to use, then you won't get the facing cut, and the very first cut will be a full stepdown distance from that Min Z height you entered. When you don't manually enter a Min or Max Z, Optirough just looks at the geometry you selected and sets the Min and Max Z to be the Min and Max extents of the geometry you want to use. Thus, if your stock model sticks above your part still, (IE, Optirough "sees" stock above your min Z) then it creates an initial facing cut to ensure that you have no possible way to inadvertently enter into stock deeper than your tool flutes can handle. 

Hope this helps!

[sendithard]

On 1/13/2022 at 2:42 PM, Colin Gilchrist said:

I don't think your Control Definition is setup correctly. You should be getting "helix" moves for the spiral down to the floor, and you should be getting "helix" moves, on each of the arcs, which connect the passes...

Can you post a Mastercam File in this thread? Strip out the stuff you don't want, but that Control Def looks like it needs to be adjusted. Both the "Arc Settings", and the Tolerances. (There is a setting where "if the helix height is less than a certain distance", it won't create the helix. I set mine to 0.00004" (40 millionths, or smaller), so I can be sure to get actual Helix motion in my NCI data.)

Colin,

I wasn't entirely sure what you were discussing here earlier. I see you can go into the machine definitions to change some stuff. The first pic below is the tolerance settings available in the toolpath parameters then the next pics are from the machine definition control area.  I'm not sure which settings you were really honing in on. Attached is my finished project to the best of my ability at the moment.

 

 

 

 

Titan_2M v3.emcam

[Colin Gilchrist]

Thanks for Posting the pictures. Set the following settings. Change your Control Definition Settings First. Then "regenerate your Operation, after changing the Filter Settings", and you should see many more "arc moves", instead of the path being broken into so many "line segments". 

I see "both the entry helix", and the "arc in/out" moves of the path, are still being broken into many small line segments. (I see this in the backplot picture...)

In the 1st Picture (Tolerance Distribution):

> Change percentage to "25%" for Cut Tolerance and "75%" for Line/Arc Filter. (Gives you "tighter output on the model [cut tol]" with better "arc fitting")

> Change "Min Arc Radius" to 0.002".

> Change "Max Arc Radius" to 4.0"

> For the "radio buttons" set to "Tighten Arc Filter tolerance" option, and slide the "slider bar" to 75%. (This says "only use 25% of the Line/Arc Filter Tolerance Value for generated "lines", and use 75% of the filter value, for creating Arcs. This attempts to give you a better combination of "straight line sections".

> Most important thing > enable the Checkbox for 'Output 3D Arc Entry Motion'. < This is important, so you get Helix moves for your cutting.

In the 2nd Picture (Control Definition Tolerances):

> Set "NC Precision" to 0.00001" (10 millionths)

> Set "Chordal Deviation" to 0.0004 (4-tenths)

> Set "Minimum distance between arc endpoints" to 0.0012 (12-tenths)

> Set "Minimum arc length" to 0.0016 (16-tenths)

> Set "Minimum arc radius" to 0.0008 (8-tenths)

> Set "Maximum arc radius" to 432.1" (Usually, anything above 200" is fine, unless you work with massive parts.)

> Set "Minimum change in arc plane for helix" to 0.00002 (20-millionths)

> Set "Maximum deviation in calculated arc endpoints from machine grid" to 0.00001 (10-millionths)

In the 3rd Picture (Mill Arc Settings):

> Leave "Arc Center Type" alone

> Set "Arc Breaks" in all three plane types to "Break at 180 degrees".

[sendithard]

Colin,

Much love for that detailed response. I'll work on that tonight or tomorrow and report back with a toolpath. That's a great post of knowledge I can put in my spreadsheet.

 

[sendithard]

21 hours ago, Colin Gilchrist said:

.

@Colin Gilchrist,

I was able to make the changes you stated. I think this looks much better. Agree?  Is this a good starting setup for mastercam in the future? 

Thanks!