I'd go with a Replaceable Drill Tip, depending on how the Casting actually cuts.

Iscar makes a line called SUMOCHAM, that go down to 8 mm in size, and increment by 0.1mm increments. You'd need a 9.3 mm or 9.4 mm drill for a 7/16-14 Thread. About 100 SFM (may need to drop down to 60 SFM, based on the interrupted cut). This is the QCP-2M Geometry. Feed Chart shows 0.08 mm/rev, or about 0.003" per Rev., but that also may need to drop a little, based on the interrupted cut.

There is the part numbers for 9.3 & 9.4 mm sizes.

That is a drill body, with cylindrical shank, thru-coolant, 12mm connection size, 3.0-L/D ratio

Here is a 8mm Milling Cutter, with 1.5/1 L/D Ratio on cutting flutes > That is a .315-Dia Cutter (in.), with .709" of Flute Length, and 7-Teeth.

This is where is gets really weird for me Steven, because I respect you, but we had maybe 10-12 sessions together at the most. I have no doubt that you spent 30 weekends in-a-row working on your Post, but not all of that time was spent with me.

Like I mentioned: you should view my MP 101 Videos & MP 301 Videos on YouTube. There is a bunch of content up there which I still believe would be really beneficial to you...

4 minutes ago, AHarrison1 said:

Just out of curiosity, why preferred?

With "Radius", you're leaving it up to the Control on how to create that Arc on the plane. We don't always get the correct interpretation, when using Radius, versus "Delta Start-to-Center" (IJK) output. IJK is also a better option for supporting Helix moves. For those reasons, I always prefer to utilize IJK Arcs, if the machine control will support it. The one drawback, you can't just "visually see" in the G-Code, what size arc radius you're dealing with. You've got to do mathematics to calculate the start/end/center positions. Since I am 99% of the time using my CAM System to full advantage, I don't care about reading the arcs as they flash by on my screen, because I've always done my work up-front in Backplot and/or Verify, to analyze the output from my Toolpaths. But I'm also always making sure I'm doing things like "Using the Toolpath filter, on each-and-every Toolpath Operation, and checking to be sure each Op is to my liking, before I'm posting my G-code.

Code is "rotated" or "models are rotated"?

I've only used Top, but had situations where I then needed to shift and/or rotate my models (done inside CAMplete typically, or I output new STL Models from Mastercam, by manipulating the model or plane, before export). That said, I would often have parts with 1 WCS, and dozens of T/C Planes.

Are you using the CAMplete Utility to output your "setup" with all the models from inside Mastercam? Once you've got your template files dialed in, and understand how to setup the GUI for the CAMplete Export, the process was seconds to export all the data for an entire setup, and launch CAMplete with that setup in the proper location on the machine table.

Well, ultimate goal is always to have the Post kick code which works on your machine, in any situation, while having to do the least amount of "Work arounds" possible. So, forcing the Plane Change on a separate line, before the new Arc, might work. However, there is probably a Parameter Setting on the Control, which affects the Plane. Are you using IJK output (always preferred) or Radius? 

14 minutes ago, JB7280 said:

I have a surface with XZ arcs.  I was trying to post the code using actual arcs in XZ, rather than segments to see if it worked any better, however, the code is posted with the G19 plane change on a G2/G3 line, which my controller doesn't like.  Is there a way to force this to change planes on a different line?

 

Am I fighting a battle not worth fighting?  Would I do better to just stick to line segments in my code??

Do you have any G02/G03 Arc Motion, in the XY Plane? If not, you should be able to force the whole path to G19 XZ output, rather than worrying about switching planes on-the-fly.

I've had to use paths like Surface Finish Contour and Surface Finish Parallel, with my Construction Plane set to Right, and my Tool Plane set to Top, to get paths like this to work in the past. Yes, you can use the Line/Arc Filter in the path to attempt to do the same thing, but you'll get the plane switching between G17 & G18/G19, and will need to attempt what you're doing now to edit the Post.

In the MP Language, there is typically a routine enabled called "Get Next Move". This function will actually "peek ahead", to give you "next move", "next operation type", or "next Tool Change" values. (The Next Tool Change values are typically used during a Tool Change or Null Tool Change, same with the "next drill cycle" data. You can do things like 'detect if the Operation is a Tap Cycle, so we can suppress the Spindle RPM, at the Tool Change before the Tap Cycle Post Blocks are called.

I bring this up because there is a variable called: 'nextplane$'. You could potentially use this to detect an upcoming plane change, and force out the G18/G19 on the linear move, which precedes the G02/G03 Arc, in case the machine does not like outputting the Plane with the next Arc Move.

Since we're on the subject of Windows Permissions, you should take Ron's advice one step further and set the permissions for:

"Shared Mastercam" & "My Mastercam" folders as well. You want the user at the keyboard to have "Full Control" over these folders & subfolders.

Pick the correct Drill Cycle in the Operation. You're using one of the cycles which isn't defined...

28 minutes ago, Bob W. said:

It isn't bad.  We keep the operators busy and we run efficiently.  Ultimately the end result is four operators generating a little under $4M per year through the machines.  It isn't just a tooling strategy to get to this.  It is the shop systems built this way from top to bottom.  The employees are paid well, have 100% health care for them and their families, 401k, etc...  Because the efficiency makes it possible.

This forum really, really, needs a "love" reaction button. 

Also, in addition to what Ron is doing, you'll want to capture that "Clearance X Value", to be able to force it out, between the moves.

With those Post Block Calls, the 'mdrill$' block is "for the 1st hole" in the series. After you've output the "first hole", all subsequent holes are output through the 'mdrill_2$' Post Block. So, copying that logic from 'mdrill$' to 'mdrill_2$', is what allows you to force out the cycle call and parameters again.

Create a Cylindrical Surface, "inside" the part you are cutting. Use the Cylinder as the Cut Pattern, and the Tool Axis Control method. Then, use "collision control" to specify "what surfaces the cutter is tangent to, as it moves over the Cut Pattern surfaces". This is known as the "clean core" method of 5-Axis path creation.

You can then choose to use "Lead" or "Lag" to push the cutter "forward (lead = positive value)", or "backwards (lag = negative value)". You could even use "side tilt" if you want, or a combination of Lead-Lag/Tilt, to keep your ball cutting on the flute, and not directly at the Tool Tip.

I find at least 4 degrees of Lead, Lag, or Side-Tilt, really improves tool life and surface quality, when cutting with a Ball. If you get get 15-20 degrees, even better, but the best results will be over 45 degrees (from about 50-70 degrees, you've got the "sweet spot" of the ball.)

I always like Harvey for small tools with corner radii.

Here is another option, with Thru-coolant, if that is an option. Mikron makes great tools, but you've got to be careful on availability. I know the tools are made outside of the U.S., and they don't always keep everything in stock. That is a place where Harvey really shines. Unless you're ordering large quantities of tools, they usually have every tool in their catalog in stock.

https://us.mikrontool.com/en/Products/CrazyMill-Cool-Square-Corner-Radius-Z2/Articles/CrazyMill-Cool-Corner-radius-Z2-Type-A-1.5-x-d

=  Equals

<= Less than or Equal to

>= Greater than or equal to

not()   < when "0" = true, "any non-zero" = false

There are all kinds of "Plane/Arc" issues to be dissected here. I'm with Zoffen > what size cutter, what kind of "lead in/out" values are you using? "Wear" is the best option. It will allow you to use a "+ / -" value, to change the size of the path. "Control" requires a larger lead in/out move, and is messy.

In addition, there are a bunch of Post Processor settings which must be setup correctly. In addition, are you using Polar or Cylindrical Interpolation? These are "options" which are controlled through a "Mill" Toolpath (mi4$), to enable "Canned Cycle" output.

The Post has specific 'scase' string settings, that control "is the Comp Code output inside or outside" the cycle.

Then, there are another set of 'scase' strings, which control the Plane Arc directions. (Allows you to swap G02/G03 output, based on which Axis Combination and Plane is active.)

This specific 'scase' string has 17 different settings, embedded and controlled by changing the 'digits' of the string. 0000000.00000000   < Each 'place' acts like a switch, where you can change the values, to flip output.

For those of you who love to geek out over "how does all this stuff work" at the lowest level, I present to you "MIT 6.172 > Performance Engineering".

What you should understand here though > Mastercam is not built around Multi-Threading. Almost every function you're used to running inside Mastercam is single-threaded. And many of the functions we are dealing with are "interpreted".

What this means is > we typically aren't using Cache in the most efficient of ways > the functions being called are simply "library functions", and we end up taking huge performance hits, because the of Cache Misses. We are constantly "running out to Memory (RAM)", Or worse, running out to "disk" (hard drive), to pull data into the Cache, so it can be processed.

31 minutes ago, JB7280 said:

Maybe a silly question, but I disabled these 3 items, and for the most part, MUCH better!!

 

However, with "Use dashed on wireframe" disabled, I don't have any indication that I'm choosing a piece of wireframe.  When using these settings is it pretty much a necessity to use the autocursor settings?

"Choosing" for selection, or to grab a "discreet XYZ position"? I believe the Autocursor is best suited to picking a "3D Point". For selecting geometry when performing a Transform, or to move/copy levels, etc., I rely on the geometry turning the color "solid yellow" to indicate the selection status. It is for this reason, that I also don't draw in Yellow, Red, or Purple (at least, I don't use the shades which are the Selection Color, Group Color, or Result Color.

On 1/22/2022 at 10:56 PM, cncappsjames said:

"... thick lines..."

 

:shudder:

 

That's a BIG negative ghost rider. 

I used to use "thinnest" for everything. Now with my eyes getting older (and being a Type 1 Diabetic), I find that the "medium" thickness is best for wireframe, while I leave my surfaces and solid models set to the "thinnest" display option. This means your wireframe geometry should be "more visible" when superimposed on top of the surface/solid geometry.

Plus, I probably don't see the behavior that annoys you, because I'm constantly "Overriding my Autocursor settings".

For selecting wireframe arc centers > hit "C" on the keyboard

For endpoints > "E"

For Midpoints > "M"

For Quadrants > "Q"

I find when I override the Autocursor settings (quick filter on an Autocursor "Type"), it is a bit easier to get the "Wireframe", rather than the "Solid Edge".

Last tip:

When I create Surface or Solid Geometry, I make sure those entities are set to "Thinnest Line Size". This property is used to show the edges of the model.

When I create Wireframe, or have existing Wireframe, I'll select it all and then set the Line Thickness to "medium". This gives me "thicker wireframe", overlaid on "thinner solid edges". It makes it easier to pick up wireframe geometry when using the Autocursor options.

2 hours ago, altamontmfg said:

Random thoughts

 

Just that little checkbox for regeneration is enough to keep me using 2022. Granted still a n00b to MC. started on 2020  BTW,

There is also Ctrl-click for selecting hole features!!! 

Instead of importing groups, I have done that, I prefer to open a file of a similar part, merge a new model and save as the new part. Maybe I just am not checking the right boxes, but import doesn't give the best results.

I also love the new Mesh Ribbon, and all the new Mesh Tools. It makes working with in-process stock, and/or Stock Flips, so much easier. I especially love the Remesh option.

The new "Unified 5-Axis" Path, and 5-Axis Auto-Deburring, worth their weight in gold. Plus, the Auto 3 + 2 is powerful as well.

Steve,

I know you're not big on trying 2021, or 2022, but try doing this, to see if it helps with your Selection issues:

> File > Configuration > System Configuration Dialog - Selection Page >

- Disable "Use glow highlighting"

- Disable "Use stipple on solids/surfaces/meshes"

- Disable "Use dashed on wireframe"

Turning off those 3 "new selection option" (eye-candy garbage to me), made the selection "like it used to be for the previous versions", and fixed a lot of my selection and visualization issues with the new versions... 

20 hours ago, Seedy steve said:

I could probably get 2017 back but I am used to this now. so hopefully I can use it until I retire.

already have to translate solid works files into parasolids to read them... I may be forced to update by something like that idk.

For what it's worth Steve, I also had problems with 2019. Mostly with the User Interface. The same kind of things you don't like, I also didn't like.

2020 was a decent improvement, and I thought 2021 was even better. (I know, once bitten, twice shy...) I like 2022 quite a bit. I feel like the team is really getting a handle on the Function Panels, and the "plumbing" under the hood.

I know you've got a bad taste in your mouth, from going to 2017 which you liked, to 2019, which you don't.

But I would seriously encourage you to take 2022 for a spin. There are a lot of really nice improvements, and more to the point > unless you're planning to retire in the next 3 years, Mastercam 2021 or 2022, could probably take you for the next 4-5 years, if you're just trying to hang on.

The decision would (of course) depend somewhat on if you're still on maintenance or not. But I would encourage you to at least go to 2021. I find 2022 to be one of the "Best 20xx Releases to date".

3 hours ago, gms1 said:

I do not like how mastercam now handles expand and collapse so I usually only create toolpath groups for each operation, never each tool. I use as few as possible.

Try this:

Click on the "Machine Group", (This puts your "mouse focus" on the Toolpaths Manager.

Now, press "E" on your keyboard. No ALT. No CTRL. Just "E"

Press "E" repeatedly.

Eventually, the Machine group will be completely "collapsed". Pressing "E" one more time, will expand all of your Groups, but keep the Operations "collapsed".

If you continue pressing "E", eventually Masteram will expand all groups and operations (plus signs). Keep pressing "E" (notice a theme here), and you'll start collapsing Ops & Groups.

The reality is this takes huge money on the Implementation and Maintenance end.

> You need to configure the software. What do you want to "do" with the data?

> You either need to pay Zoller to implement your system, pay a 3rd Party Integrator to do it, or pay someone on your company's internal staff to do it (like Zoffen suggested).

> How do you want "data" to flow?

> Who is maintaining your software & your databases? Who is maintaining your Tool Crib Inventory?

JB has attested to the same thing I've seen in other shops with Zoller. They use the equipment for a fraction of "what the system could do", and they use the Presetter to set tool lengths, and print out labels, with Tool Length and Diameter values. The "label" is attached to each Tool Assembly, on a Tool Cart, which is parked next to the machine. The next job comes up, and the Operator unloads all the old tools, and manually loads the assemblies into the tool magazine, and then enters all the new TLO and Diameter Offsets "by hand", at the control.

I've seen other shops where this Tool Data was written to an RFID Chip. At the machine, there is an external "tool registration" station, where you scan the RFID tag. This automatically loads the TLO CRC values, without the possibility of operator error. However, the Operator could still accidentally load the wrong tool in the Tool Pot. The only way to really "close the loop", is if you have the ability to assign each Tool Assembly a unique identifier, and then have a "read/write data head", which can engage the tool while it is in the spindle. (Usually a data read/write event, before/after the tool is used. This does add some extra time, but results in process security and reliability.) The problem is > someone has to design the system, integrate all the hardware into the machines, train everyone how to use it, and then hold them accountable.

That last part, is typically the hardest.

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".

37 minutes ago, Afshin karimi said:

• Thank you. That's what I was looking for. appreciate it

You're welcome, but keep in mind this is for Surface Finish Contour path only. You'll need to generate a "surface" for the boss. Not a big deal, but there is no option for this "start Length" when driving Wireframe Geometry with a 2D Contour path.

To control "Depths" with SFC, you need to use the "Cut Depths" dialog box.

> Press the [Cut depths...] Button

Now, there is a bit of a secret here. For "Incremental", you have Adjustment to Top Cut, and Adjustment to other cuts.

> For "Adjustment to top cut", A Positive Number tells your cutter to "drop" that amount below the very top of the detected surface. Positive Number = Negative Depth (for this control only)

> For "Adjustments to other cuts", that values works the way "you think it should". A Negative Number = Negative Depth Adjustment. A Positive Number = Positive Depth adjustment. If you're depth cut value is "0.05 inches", and you can visually see you want to make "3 passes deeper", you'd subtract from the value. (if it was 0.0, change to -.150, to force 3 more depth cuts.)

This "Adjustment to Top Cut", is one of the weirdest, and trickiest options to understand in using any toolpath in this software. I think this is why so many people have switched over to "Absolute" values, when using Depth Cuts, for Surface Finish Contour. The problem is, if you end up changing your Plane or Geometry Depth, in any way, you've got to go and edit all the paths which use "Absolute" values. If you learn to properly use "Incremental Depths" (For both 2D Ops and 3D Ops in Mastercam), you have a lot more freedom to make a "global program change", where you can safely move an origin point, and all the Operations will regenerate without manual intervention.

In general, I'm a big fan of adding Groups and Subgroups to organize your Operations Tree.

I will only add a "new machine group", when the "part physically moves to another machine". My tree looks very similar to John Paris' Tree above.

> Machine (only changes, if part "physically moves" to another machine)

    > OP 10 (or OP1, depends on your numbering convention. Aerospace tends to use increments of '10'.)

       > Tool 1

       > Tool 2

       > Tool 50 (etc.)

   > OP 20 (or OP2): We create a new "main node" under the Machine Group, any time a new WCS is used. (Part flips from 1st location, to 2nd location [vise], etc.)

       > Tool 1

       > Tool 2

       > Tool 3

How you organize your tree will depend quite a bit on the "type of work and machines" you are working with. For example, in John's Tree above, he is adding "extra subgroups", after the Tool Number, to indicate "which Work Offset Location" he is cutting at. This is because you might have "the same tool number", being used on multiple sides of a Tombstone.

> MCH

    > OP #

         > Tool #

               > Plane and/or Work Offset Number (basically > the location where the cutting is taking place.)

Now, I will also sometimes "break my convention" if there is a good reason for doing so. For example, I will sometimes create a group for a specific feature:

> MCH

    > OP #

        > 1/4-20 Tapped Holes

Now, in this "1/4-20 Tapped Holes" Group, I would typically have at least 3 separate Operations. One for each Tool being used, but typically 3 Ops. 1 = Drill, 2 = Tap, 3 = Chamfer.

For me, the deciding factor is "do I need to use these tools for any other work on my part, besides tapping these holes?"

> Why?

Because the tools I've put under that group are all related to the same feature on the part. Otherwise, you end up with "3 groups", each with a single operation underneath it. I'm not a fan of that.

For other parts, I will sometimes do something like this:

> MCH

    > OP #

         > ROUGH

            > T1

            > T2

            > T3

         > SEMI-FIN

            > T4

            > T5

         > FINISH

            > T6

            > T7

            > T11

            > T8