[jrmach]

So I made 5 pieces of this part today.
First of all,as we all know,things are different at the machine than the Computer screen.Little things present themselves and of course big things sometimes.Stuff that just don't quite get your attention until you see and hear the cut.
So with only 5 pieces to do,,,Time running the part is not extremely important.So I ran the part,less than ideal.I just Babysitted the machine and played with the feed over ride when needed.
But now that I am in the comfort of my house,I wanna learn from my sorta un-productive tool path.
I choose Adaptive Rough with a Parallel Pattern.Actually,to me it is a bad ass too path for this part,EXCEPT for one thing.The first pass at each level is a Full cut.This creates too much feed for this cut vs. the cuts that come next.Hence is why I Babsitted the machine.
So,am I missing something ?
It sure looks like the right path,just need one of those "mmoe" buttons to say slow down first pass on each level.If I had a quantity of parts I would definately choose this path and just edit the code.It really kicked butt.Unless of course someone has a better way I'm all ears and eyes,lol


I really hope you see this mmoe I would like hear your opinion of this and/or what I should of done differently.I still have to run the other half with the same kind of geometry.
And I welcome all thought from everyone.

This is just a example of the actual file I ran today,,,btw I finished with Equal Distance and with a little tuning of the diameter and radius of the EM,I nailed this part on the money.This part holds a hydraulic ram in place and also positions it in all axis for mating assemblies,,,so I was pleased.

[SBC Cycle]

So I wouldn't have to babysit:

Rip down the middle with a slow feed all the way to depth. (Just a 2D line and toolpath, connecting the middle of the end arcs)

Run simulation and save the stock.

Load new "roughed" stock as material in the Stock Wizard (.stl)

Extend your boundary in the X axis about 0.500" in both directions. Re-select the boundary.

Change the Advanced Rough pattern to "Offset" and recompute.

Post code and walk away.

This is one of the reasons I want to update to V27. I want each feature to use it's own "stock", or basically recognize the material removed by the previous feature. I think V27 has that ability of some kind, if I recall. What would be even better is if the toolpath had an option to recognize the first cut, which is always going to be a full diameter cutter engagement at each depth the way the toolpath currently works. I know what you are saying about having to babysit. I can edit the code to slow down on that first full engagement cut but I'd rather not.

[jrmach]

So I wouldn't have to babysit:

Rip down the middle with a slow feed all the way to depth. (Just a 2D line and toolpath, connecting the middle of the end arcs)

Run simulation and save the stock.

Load new "roughed" stock as material in the Stock Wizard (.stl)

Extend your boundary in the X axis about 0.500" in both directions. Re-select the boundary.

Change the Advanced Rough pattern to "Offset" and recompute.

Post code and walk away.

This is one of the reasons I want to update to V27. I want each feature to use it's own "stock", or basically recognize the material removed by the previous feature. I think V27 has that ability of some kind, if I recall. What would be even better is if the toolpath had an option to recognize the first cut, which is always going to be a full diameter cutter engagement at each depth the way the toolpath currently works. I know what you are saying about having to babysit. I can edit the code to slow down on that first full engagement cut but I'd rather not.

Thanks SBC,
Yet another way to add to the arsenal

What gets me with decisions like this is the "Quantity" of parts.
I don't play with actual code hardly ever,so I am real slow editing.And then I got to be careful and prove it.(I rarely ever Dry Run,I depend on Preditor,Experience and over rides.Just press go)
or
I can go to the Extra trouble and program in a way like you say(and I just may with the mating parts I still have to make),but that takes time,and sometimes a lot of time to learn and figure it out
or
I can quickly code like I did here and get it done.Stand there over ride the feed as necessary.Only 5 parts.When I say Babysit,there really is nothing else to do as all my other machines are at home.I can Computer,it is like 4 feet away,not so bad...

And then there is always that looming question,"can i make it faster on Manual Machines?"And since it's all about getting paid doing whatever is fastest,I do a lot of Manual Machining sometimes for onesy,twosy.
Sounds like you would like a button too?

And I just was telling mmoe to be careful what you wish for as far as feature requests.So now here I am and want another button too.I will eat Crow if have to,really hope mmoe does respond,I want more opinions right at the moment.That goes for anyone that may have a voice on this.
Glad you picked-up what I was talking about.These little things come out about the time the EM touches the metal.Luckily with a %50 feed over ride at first running.I was only holding on to 1/8 inch of material and HSS is all I had to cut with,so slower feeds anyhow..I did not see that ahead of time,But now I know.
I still think for down and dirty this was good.It was fast to program,efficient,and great on the cutter,if not for the full cut.I would like a button,what do you say mmoe ?

[jrmach]

Extend your boundary in the X axis about 0.500" in both directions. Re-select the boundary.

I should explain,,why I didn't do that this time.Cutting with a Ball and with the 20ipm rapid down and the Boundary set as I did it,and a doc of .150 and step-over of .150 and the feed of 40 ipm,,It all just blends in as a fluid cutting tool path.Like a X,Z arc/ramp entry kind of,at least sounded all good.
I do see why to do this though and have mysefl at other times,thanks

[jrmach]

Rip down the middle with a slow feed all the way to depth. (Just a 2D line and toolpath, connecting the middle of the end arcs)

Run simulation and save the stock.

Load new "roughed" stock as material in the Stock Wizard (.stl)

Extend your boundary in the X axis about 0.500" in both directions. Re-select the boundary.

Change the Advanced Rough pattern to "Offset" and recompute.

Post code and walk away.

That looks to work pretty nifty Mate,at least on the simulator.Still would like a button,but I see nothing wrong with this way except it is some more work and you have to have knowledge,,I thank you for the latter.
I have used the saved .STL a few times.They give my laptop quite a work-out.This one not so bad,but still feel the extra weight here.

[mmoe]

I did a heat press caul for a client in aluminum a couple months ago that was just essentially a larger version of what you have here, but also more of a parabolic shape than round. Since it was just an extrusion of the parabola across the part, it's essentially the same concept. I think that to a great extent, how you approach things depends a little on your equipment and the material you're cutting. My machine must move VERY fast while cutting, especially if I'm using a 3 flute tool since I have a hard time getting my spindle below 10,000rpms (the amps really start to go up as you approach 7500rpms, which means lots of heat on the bearings and windings). While I can machine with a full 10hp if needed, I sure don't want to do so at 110volts, which is what a VFD would try to do if I drop the RPMs like that. With those machine limitations in mind, I have to keep my machine moving as fast as I can and the adaptive strategies play into the strength of the machine that way.

The other thing I usually have to do is give my machine time to slow down and change directions. I have pretty old DC servos (circa 1990) that just can't go from 300 ipm to 0 and back to 300 ipm the other way in less than an inch or two, but I want to ensure that the spindle speed and feedrate are both stable when the tool hits the part on the finish pass. To allow for the somewhat crappy acceleration/deceleration, I create an expanded surface to generate the finish pass on. The part in the photos below is about 5 inches long, so the total length of the surfaces for the finish pass is around 8 inches long or so.

On a smaller part such as yours, I probably would still prefer an endmill for roughing over a ballmill. I don't like the stair steps left by an endmill, but at the same time I haven't really ever had them be a problem either. I actually like SBC's approach for a part like that, though I would add that I may line them all up if you can fit them in a vice at the same time. I might even expand on what SBC proposed and use an adaptive strategy to create a narrow slot by using a narrow boundary just a bit wider than the tool. It's painful to watch the machine do it, but it can create a full depth slot nearly as fast as it could running straight, but without full width tool engagement. I also only machine aluminum, so I don't really know how dealing with steel or iron affects the choice of cutters or approach. A ballmill for roughing in aluminum (my only point of reference) seems like it would probably gall up quickly even in nicer aluminums (7075 or 2024), so I have a hard time knowing how it would handle steel/iron. I'm hoping to get a VMC later this year (probably a fixer upper), so I'll have to find out soon enough and I'm sure I'll be asking a bunch of pretty obvious questions about coolants, spindle speeds and bits.

I can't share a file in this case, due to client's wishes, but I can show a photo so long as it's not identifiable what the caul is used for specifically. Very similar part to what you're doing.

[mmoe]

BTW, I really want to try V27 on this same part, which I'll have to do in the near future as the client needs more fixtures. I had to space the Slice Planar tight to allow for the vertical areas to get machined well, but now with "Advanced Planar", I can space the flats better and still get tight step overs on the steep areas. I have a feeling that V27 will save about 3 minute or more on each of these parts.

SBC,
I'm not sure about the stock in V27. I haven't noticed it behave any differently than it did in V26. I'll have to look into that and see. Could be I just haven't paid close enough attention.

[SBC Cycle]

mmoe,

In V27 it's called "Operation Stock" or "Trim to Stock". It will override the Stock Wizard stock for just that feature. That's the same thing I do in V26 but I do it manually. It's similar to rest roughing but less automagic.

The Adaptive can be a little slow sometimes on parts like this because it's doing exactly what it's supposed to do - avoid a full engagement of the cutter. I would rather it work like you suggested: mill just a narrow slot using the loop - loop - loop High Speed strategy, THEN apply the Adaptive to the stock that's left. A lot less looping around and cutting air.

I'm finding a hard time putting my thoughts into words this morning, too many holiday "spirits" last night, lol. Hopefully you understand what I'm saying.

jrmach, I agree with you that a "button" to slow down the first (full engagement) cut would be nice and it doesn't seem like it would be a difficult task on the software side. I understand why you did what you did, given the way it works currently. I only extended the boundary out to give the Advanced Rough some room so it wouldn't try to feed down into the stock (since I removed the center portion manually with a 2D toolpath, it's wasted movement).

[SBC Cycle]

The other thing I usually have to do is give my machine time to slow down and change directions. I have pretty old DC servos (circa 1990) that just can't go from 300 ipm to 0 and back to 300 ipm the other way in less than an inch or two, but I want to ensure that the spindle speed and feedrate are both stable when the tool hits the part on the finish pass. To allow for the somewhat crappy acceleration/deceleration, I create an expanded surface to generate the finish pass on. The part in the photos below is about 5 inches long, so the total length of the surfaces for the finish pass is around 8 inches long or so.

I do the exact same thing as this with a very similar "half pipe" part we make. My VMC will try to reverse on a dime if in G01 feed mode, it won't slow down for sharp corners or severe axis reversals without some specialized code. Instead I extend the surface outside of the part and manually add a "G09" (exact stop or "ramp" mode) before the feature. Then I can run 300IPM or higher and it will coast to a nice, soft stop, move over, and take off at a controlled acceleration again in the opposite direction. No dwell marks on the part or blemishes from the linking moves to deal with.

[jrmach]

mmoe,sounds like aluminum would even be pain in your machine,on top of what you listed you have no coolant.
All I had was HSS cutter in ball form.You run that a 10,000 you will be welding.
I only run 1 part at a time,,only 5 pieces.I also finish the part for that side complete.I also only have .125 to hold on to,,and it is not a machined surface on 1 side,just a saw cut.So 1 part per vise.
I find Equal Distance is better compared to splice planar.You have to have such a small step over with splice planar in this configuration.Equal distance cut a little more air,but was real satisfied for the tolerance and fit of the part.I used a .035 step-over.with 75 feed for that.
For the adaptive rough,After the first full cut,I over ride it to 80 ipm jsyk.3900 rpm with flood coolant is highest speed you dare go with a 1/2 ball HSS,,mmoe,I have no idea if you indicating you would go 10,000 or if you would of been screwed and could not run that cutter?
I use to have a couple Carbide Balls,but wore them out in steel,,I may order a Carbide ball today so I can quit fiddle farting around and shave %60 run time or better off the top ? It would be probably worth it as I will bee running this job in a few more months again.Some day I will post my collection of tools,it's crazy the amount I have for a one man show.Sure some of you understand that.

So mmoe,should I feature request a button,,or are we good how it is?My only objection to SBC idea is my inferior laptop pukes when using saved .STL files.It always works,but not fast and certainly without looking like it crashes at first.
That,and it is a little more programming work.I will PM address where to send Crow to if needed


A ballmill for roughing in aluminum (my only point of reference) seems like it would probably gall up quickly even in nicer aluminum
It is a whole new game with flood coolant.Everything you thought you knew about cutting aluminum will have to be changed.Not talking mist/talking a flood.Not talking You Tube video's either,as they usually turn it down or off so you can see.I am talking a FLOOD.SBC has a fire hose on his HAAS I am sure.
without flood coolant and slower speeds available when needed.,it don't matter what kind of aluminum,you will be welding.
On my machine I have 10,000 rpm max with 20 HP.So,if I was using a 1/2 Carbide Ball,,I would go 9000 rpm.I almost always leave %10 off the top rpm,as I hear it is just good practice to not strain your machine.Wife's Tale,I don't know,,but I just put a new spindle in last year that cost over $4000 and I had to pay for it,suks.
JSYK,,,2024 cuts like a butter,,it is my favorite.Softer,but stronger than 6061About 2X the price though.
7075 is almost like mild steel as far as hardness.On the lathe,it can be a right pain in the ass until you get everything set up right.Stringy,stringy chips.It has the most tin content added as far as the basic aluminum's go.7075 is the strongest and it is by far the one that Buffs like Chrome the best.Also resists oxidation (dulling) the best after it is buffed.Also is resistant to scratches.Parts that need strength and Bling I make from this.Also cost 3 to 4 X as much.
Cast aluminum suks for anything but mic plate
6061 is the most common series out there,But beware depending on heat treatment type and specs,,some of it is weak as heck and Wood be better.Thankfully most out there is T6511.This is what I use %90 of the time.
3000 and 5000 series are mostly in sheet form.

[jrmach]

BTW, I really want to try V27 on this same part, which I'll have to do in the near future as the client needs more fixtures. I had to space the Slice Planar tight to allow for the vertical areas to get machined well, but now with "Advanced Planar", I can space the flats better and still get tight step overs on the steep areas. I have a feeling that V27 will save about 3 minute or more on each of these parts.

SBC,
I'm not sure about the stock in V27. I haven't noticed it behave any differently than it did in V26. I'll have to look into that and see. Could be I just haven't paid close enough attention.

Please report back

[mmoe]

Here's a quick comparison of the "Advanced Planar" and the standard "Planar Slice". I made the toolpaths match in terms of the distance between stepovers on the steep portion of the cut. In the standard version, this is a .2mm step over, which generates something more along the lines of a .5mm (.020" or so) stepover on the steep areas since it projects the .2mm spacing down on an angle. If I use this standard toolpath, I end up with .2mm spacing on the flats, which is a lot of unnecessary passes if I feel .5mm is good enough for the surface finish required. In theory, a .5mm spacing with a 9.525mm (3/8") ball-endmill will produce a surface deviation of .006mm or .0002" between passes. What would be ideal is getting around a .5mm spacing on the flat surfaces while getting a .5mm spacing on the steep areas as well. You could do this in the past by breaking it down into several regions and creating individual toolpaths, but it really didn't have a good transition from one area to another particularly when there is a transition from steep to flat at the bottom of an arc as we have in these examples. The new "Advanced Planar" basically provides exactly what is needed to get the kind of spacing you like from Equidistant Offset, but keeping the back and forth motion that is more efficient as well vs. the loops that Equidistant produces. Also, Advanced Planar now has arc/spline links between each pass to make the transition from one direction to the other a little smoother, but it also makes that transition past the edge of the part surface instead of the "follow" option that you get in the standard strategy.

For the Advanced Planar, I found that I can set the regular step-over to .5mm instead of .2mm, then set the adaptive "minimum stepover" to .2mm. This produces about the same .2mm spacing on the vertical areas which produce an equivalent to .5mm step over (again because it's projected down onto an angled face) as the .2mm stepover in the standard Planar Slice, but also allows the stepover to be .5mm on the flat areas. On the flat areas, this saves more than 50% of the cutting time vs. a single Planar Slice strategy. For every 10 passes on the flats by Advanced Planar, Planar Slice takes 23 passes, while in the steep areas they match up exactly the same. To me, this is a huge time saver whether you choose to save your time at the programming stage or the machining stage. Either way, a similar level of finish quality used to take longer to achieve. You can basically get a Equidistant Offset quality finish without significant increases in machine time while also getting the benefit of a parallel pattern which is often much more efficient than the loops that Equidistant Offset likes to produce. Not to mention there should be fewer opportunities for dwell than I get from Equidistant Offset. I'll still be using Equidistant Offset for a significant portion of what I program, but I now will match it to curved shapes while more linear shapes will get Advanced Planar. There is also an "Advanced Z-Level", but I really have not found that one very useful yet. I've never used Z-Level machining for anything but roughing, just haven't been a fan of that strategy for finishing passes.

In the image attached, the green is the "Advanced Planar", while the red toolpath is "Planar Slice or Slice Planar" (can't really remember which it used to be called, and now it's just called "Planar"). You can also see the spline connections between passes on Advanced Planar, while the standard Planar is set to "follow".

[mmoe]

mmoe,sounds like aluminum would even be pain in your machine,on top of what you listed you have no coolant.
All I had was HSS cutter in ball form.You run that a 10,000 you will be welding.
I only run 1 part at a time,,only 5 pieces.I also finish the part for that side complete.I also only have .125 to hold on to,,and it is not a machined surface on 1 side,just a saw cut.So 1 part per vise.
I find Equal Distance is better compared to splice planar.You have to have such a small step over with splice planar in this configuration.Equal distance cut a little more air,but was real satisfied for the tolerance and fit of the part.I used a .035 step-over.with 75 feed for that.
For the adaptive rough,After the first full cut,I over ride it to 80 ipm jsyk.3900 rpm with flood coolant is highest speed you dare go with a 1/2 ball HSS,,mmoe,I have no idea if you indicating you would go 10,000 or if you would of been screwed and could not run that cutter?
I use to have a couple Carbide Balls,but wore them out in steel,,I may order a Carbide ball today so I can quit fiddle farting around and shave %60 run time or better off the top ? It would be probably worth it as I will bee running this job in a few more months again.Some day I will post my collection of tools,it's crazy the amount I have for a one man show.Sure some of you understand that.

So mmoe,should I feature request a button,,or are we good how it is?My only objection to SBC idea is my inferior laptop pukes when using saved .STL files.It always works,but not fast and certainly without looking like it crashes at first.
That,and it is a little more programming work.I will PM address where to send Crow to if needed


A ballmill for roughing in aluminum (my only point of reference) seems like it would probably gall up quickly even in nicer aluminum
It is a whole new game with flood coolant.Everything you thought you knew about cutting aluminum will have to be changed.Not talking mist/talking a flood.Not talking You Tube video's either,as they usually turn it down or off so you can see.I am talking a FLOOD.SBC has a fire hose on his HAAS I am sure.
without flood coolant and slower speeds available when needed.,it don't matter what kind of aluminum,you will be welding.
On my machine I have 10,000 rpm max with 20 HP.So,if I was using a 1/2 Carbide Ball,,I would go 9000 rpm.I almost always leave %10 off the top rpm,as I hear it is just good practice to not strain your machine.Wife's Tale,I don't know,,but I just put a new spindle in last year that cost over $4000 and I had to pay for it,suks.
JSYK,,,2024 cuts like a butter,,it is my favorite.Softer,but stronger than 6061About 2X the price though.
7075 is almost like mild steel as far as hardness.On the lathe,it can be a right pain in the ass until you get everything set up right.Stringy,stringy chips.It has the most tin content added as far as the basic aluminum's go.7075 is the strongest and it is by far the one that Buffs like Chrome the best.Also resists oxidation (dulling) the best after it is buffed.Also is resistant to scratches.Parts that need strength and Bling I make from this.Also cost 3 to 4 X as much.
Cast aluminum suks for anything but mic plate
6061 is the most common series out there,But beware depending on heat treatment type and specs,,some of it is weak as heck and Wood be better.Thankfully most out there is T6511.This is what I use %90 of the time.
3000 and 5000 series are mostly in sheet form.

I use mostly 2024 aluminum and steer customers away for 6061 and similar as much as possible. As you point out, I don't have coolant, so anything other than 2024 or 7075 cut very poorly unless I can keep the chipload a little on the high side. When you are running 10k-15k rpms, that means some pretty serious feedrates that can look a little on the scary side. When cutting aluminum dry, conventional cuts are complete garbage in my experience, no matter how light I take them, so I really try to keep the tool in an adaptive pattern running climb mill only. I can get a very nice finish off of 2024 without a whole lot of trouble and 7075 machines pretty easily as well with a little bit of WD-40, so I tell my clients that it will save them more in machine time than the additional cost of the material vs. using cast or 6061. I use pretty much carbide only for tools, again due to the way my machine works. Even at the prescribed feeds for the spindle range I can run in, HSS tools just burn up. Some of the coated tools do a good job of preventing the welding/galling in 6061 even when I'm spinning them at 15000 rpms with a light coating of WD-40 on the part surface.

I agree on the spindle RPMs. I never run mine at full speed. Technically, mine should run up to 20,000 rpms, but I never exceed 15,000. Those I have known to run their spindles full speed tend to replace/rebuild them a lot more often. May be a wive's tale, but there is plenty of evidence that says it's better to keep them in a narrower range than they are spec'd for.

I do think you should submit a feature request that full width passes be treated differently. I think they also need to do a better job of identifying those places where it occurs in the "rest machining" conditions. In those cases, you are often using a smaller tool that is more likely to break, so you really don't want a full width pass! Yet that's were I encounter it the most.

Do you know anything about Cincinnati VMCs? I just passed on one a couple weeks ago for $3500, which needed some control repairs (I have no problem doing that myself and have retrofitted many machines now). I just wasn't sure how good the machine is even when it's working well. Haas seems to be the mainstay for most shops, but others like Cincinnati seem to be easier to find a good deal on a fixer. Are there any brands to avoid?

[jrmach]

If there is any significant amount of material to remove,I never conventional cut.
Only tome I conventional in a manual mill is with corner rounders or other form tools.I use EM,even roughing in manual mills with a Climb cut.I don't suggest anyone try that unless you are real familiar with a mill,because there are tricks to accomplish this.
My go to cutting oil for aluminum is A-9 by Relton.$34 a gallon.This is good on plastics too,not steel though.The stuff even smells good.Seriously,try it.It also cleans up nice and easily.
Best EM I found on Aluminum,hands down are Alu-Power Alumpower end mills | eBay They are outstanding.Leave like a 16 finish,no kidding,mirror shine.I use them as finishers.Can't recommend them enough for Aluminum,especially with no coolant.I use them both in CNC and my Manual.
As far as knowing CNC's,,,well I want ones that cost too much,lol
For one on a budget,but yet big enough to not be a Toy,,my limited knowledge would recommend a HAAS or Fadal.My reasoning is they are both reasonably priced used and you will be able to get parts for either one as long as you will live.It is true Fadal is out of business,but don't let that deter for one minute.They have an after market business like no other.There is actually a company here in Boise that actually refurbishes and makes parts for the old fadals.They are both highly supported by technicians/mechanics if need be.
SBC owns both,he should be able to comment further.
The old Cincinatti, CNC'sI heard are kinda clunkers.Just what I heard.However their old manual machines are 2nd to none.So I really cannot give you a reliable answer.
Spending $3500 only,,,reads buyer Beware.

[Besel@bobcad]

Attachment 262196

jrmach,

I'm not sure if this has been answered yet in another one of the posts in this thread or not. I figure I'll put the answer up and then go through these in between tickets lol. Anyway to avoid the full cuts through the material, I did two things to your part. 1) Selected the Adaptive Roughing option in the Patterns screen..... This got what we wanted but it did start ON the material. Once it bit into the material it started a slow spiral out with constant engagement. The only reason it started ON the part was that you were using a boundary to force it to stay on, which brings me to number two. 2) removed the boundary from the feature and recomputed. I think this is more of what you were going for. Hope this helps.

[Besel@bobcad]

SBS Cycle,

Yes. Version 27 DOES use individual bounds for all of it's 3D operations (since you can use multiple operations in a single feature) and individual stock options for several of the new 3X Pro features. This is one of those upgrades that is a MUST!..... You guys are going to love it! If you have any questions, please feel free to give tech support a call. 727-489-0003

[Besel@bobcad]

Attachment 262198Attachment 262200

mmoe,

Speaking of stair steps left by the endmill, make sure that you guys utilize the Intermediate Steps option in the Advanced Roughing. In V27 we've even added a way to set the ORDER of how those steps are handled!

[Besel@bobcad]

jrmach and mmoe,

Wanted to let you guys know that I've put a feature request into development on your behalf to have a way to set, or have the software automatically set, a slower feed rate in the areas that the tool will engage the material fully.

Let me know if you have any other questions or need anything else: 727-489-0003 or email [email protected].

Happy Holidays guys!!

[jrmach]

Thanks for the very fast response.
A way to control the feed in that first pass will speed the tool path up significantly.Hope it makes the next update/upgrade.
Will be upgrading as soon as money allows,,there is just too much new "Kung Fu" going on to not.Especially this SBS Cycle,

Yes. Version 27 DOES use individual bounds for all of it's 3D operations (since you can use multiple operations in a single feature) and individual stock options for several of the new 3X Pro features. This is one of those upgrades that is a MUST!..... You guys are going to love it! If you have any questions, please feel free to give tech support a call. 727-489-0003