Surfcam Truemill?

[esherbro]

Wow, lots of great questions. I'll see if I can respond to some of them.

 

First of all, to Jeff, I don't unfortunately have access to the SDK for Mastercam 9, so I can't make a version for it at the moment, although I will look into the possibility of getting a copy. I am in the process of backporting it to some versions of X, however, and hope to have that out soon. In the meantime, you might find our Universal Client useful; it takes a DXF file of the part boundary as input and posts G-code out directly.

 

Mic, to answer your questions, TrueMill keeps what you might call a "bounded" engagement angle, so that the engagement angle is never greater than a specified value. It can be (and often is) less than that engagement angle due to the requirements of the toolpath. VoluMill actually does not have a constant feedrate; it's adjusted when necessary to keep the material removal rate as close to constant as possible. This means, for example, that it will slow down slightly when entering ccw arcs in climb milling, but it doesn't have to slow down a lot because the toolpath never turns very sharply unless it absolutely has to on the final pass when negotiating a tight corner.

 

Unlike TrueMill and adaptive clearing, VoluMill does not currently use looping trochoidal-like motion to open up pockets. Instead, if necessary, it uses multiple axial depths to open up new areas. Even though it fully engages the tool, by reducing the axial depth and removing corners from the fully-engaged cut it is still able to move quickly in these areas. Your point about making actual demo g-code available is an excellent one, and we are actually working on doing that right now through our website. I'll keep you informed. In the meantime, you might want to play the sample video on our site to get an idea of how the toolpath works; it shows what I'm talking about pretty clearly, I think.

 

To answer your question about why it is better, I guess the short answer is that TrueMill is sort of an intellectually pure solution and has some drawbacks as a result. Don't get me wrong, I'm proud of the work I did making TrueMill, and it is still making a lot of Surfcam customers very happy (and saving them a lot of money), but it has some inherent inefficencies due to the need to keep tool engagement strictly controlled. The biggest symptom of that is the amount of air-cut repositioning that occurs because of the looping cuts. Our approach seems typically to lead to the tool being in the material a larger percentage of the time, and a shorter overall path length while being able to run at similar speeds.

 

Colin, let me see if I can answer some of your questions. I have a couple for you as well. You're quite right that if you no longer have a subscription you won't be able to regenerate a toolpath unless you reactivate the subscription. I guess the flip side of that is that if you are using the service that infrequently, it's much cheaper to have a subscription that you can turn on or off instead of an application that is basically shelfware most of the time and cost a lot of money up front. The internet does go down from time to time, which is a risk, but seems to be a very small risk these days, at least in my experience. Even if the internet goes down for a few minutes, the Mastercam client will allow you to program the part and just leave empty toolpaths that can be regenerated when connectivity is restored without the need to reset parameters or geometry.

 

Your question about processing time is an interesting one, and I'm not sure I understand it fully. I actually view the remote processing as an advantage rather than a drawback. Given a choice between calculating a complex 3-axis toolpath locally on a single desktop machine versus calculating remotely on 20 servers running in parallel, each of which is an order of magnitude faster than my desktop machine, I would choose the remote calculation and 200x speed improvement. We do not yet have our 3-axis service running, but we anticipate this will be a key feature. With the remote calculation, there might be a hit purely related to data transfer to and from the server, but with compression and broadband I'm guessing this won't be much of an issue. We've done some stress tests of this nature with our service and we haven't even noticed the transfer time. It's possible, though, that I did not understand your point correctly.

 

You are right that many people are simply not on maintenance any more; the percentage I'm sure varies from company to company, but I seem to remember that on average, slightly higher than 50% of customers of the major midrange CAM companies are on maintenance. Interestingly, I've heard that it's significantly higher with SolidWorks for whatever reason. We guessed, possibly wrongly, that most off-maintenance customers would be happy with what they have and would not necessarily be that receptive to what we have to offer, whereas customers on maintenance are used to monthly or yearly recurring fees and might appreciate the fact that they don't have to pay a bunch of money up front to get started.

 

We'll do our best to keep an open mind, though, and I really appreciate your comments. Thanks!

[Guest CNC Apps Guy 1]

quote:

---

...I've heard that it's significantly higher with SolidWorks for whatever reason...

---

It's because if you don't maintain SW, you loose the ability to collaborate with outside companies that ARE using the latest stuff AND you'll end up having to re-"purchse" at full price after a fairly short period of time.

[Mic]

Hi esherbro

 

Thanks for answering my question's.

 

About this ramp opening for new area's. For aluminium it will work fine, but for harder material I would still prefer the TrueMill approach. Imagine a long and narrow pocket. Here would TrueMill make a helical opening and then open the centre of the pocket with trochoidal and that way use the side of the tool for most of the material removal. VoluMill would ramp out the centre part and that way cut much more material with the bottom of the tool instead of the side.

 

I've seen your video ( please make the next one without coolant as it will make it more easy to what's going on ) and the motion looks very nice and smooth. But now I need 3 different software's. MasterCAM for all basic stuff. VoluMill for roughing aluminium and TrueMill for for roughing stainless, titanium and other hard to cut material's.

[mold100]

I use surfcam truemill for roughing aluminum in 2d i do not care for the 3 axis path. The 2d is by far the best high speed 2d roughing i have used as of yet. 1.25 deep pocket 13in long x 9 in wide with a .500 cutter in 6 minutes flat and that was not pushing it, less than 2 inutes to grab chain program, and post.

 

On the other hand that, drilling on center line and ease of work cooridinate setting are the ONLY 3 things I like about surfcam. Mastercam is far more superior out of the box with no add ons.

 

James,

 

That is is one of the very few reasons I keep my Solidworks maitenence, customers. If I am not up to date I dont get the file.

 

Sorry for somewhat of a high jack.

[gcode]

quote:

---

you'll end up having to re-"purchse" at full price after a fairly short period of time.

---

At the rates SW charges for maintenance (25%)

you "repurchase" your Solidworks every 4 years

They make very good software, but they are a pack of thieves and I tell them so every time they send me a bill. I also have issues with Solidworks about Catia translators.

You can open nearly every CAD file out there with SW except SW's big brother Catia. For that

you must buy a translator.

Two softwares from the same company and they can't talk to each other.. and the only reason is greed.

Still.. the software is good enough that I put up with thier BS and write the checks

 

sorry for the hijack

[esherbro]

Hi Mic,

 

Sorry, I may not have been very clear about the way new areas are opened. VoluMill does use a ramp entry (with no corners, it's kind of like taking a helix and stretching it out to a sausage shape) to get into a closed pocket initially, but any subsequent area that needs to be opened is opened with multiple depths of cut where the z value is constant for each depth, so it's not a ramp. So although less of the axial depth of the tool is engaged, it is true side-cutting, not cutting with the bottom of the tool.

 

We do intend to offer the option of a helical entry instead of the initial ramp entry, but our tests to this point indicate that the ramp entry tends to save a lot of time. Often with a helical entry you have to do many passes because you don't want your z value to change too quickly; with the ramp entry you can often get to the bottom in fewer passes at a shallower angle than your limiting angle, and the path length is much less than doing the helical entry and then opening the rest of the area up.

[esherbro]

CNC Apps Guy,

 

You're absolutely right. The need for collaboration drives a lot of maintenance revenue, and that need seems to keep going up every year.

 

This is one reason that I would not be surprised to see more subscription models in the CAD/CAM industry. In some ways, it's a natural evolution from purchasing software outright, to regularly purchasing upgrades, to enrolling in a maintenance program, to enrolling in a subscription service.

[esherbro]

mold100,

 

Since I worked on the 3-axis version of TrueMill, I probably owe you an apology. You are right, it is nowhere near as good as the 2-axis version, and that has more to do with internal problems at Surfware which I am not at liberty to go into than with the underlying technology. You can sort of view it as the initial version of something that was going to be much better in a later release but was never improved. For example, if you use it to rough out the cavity of a bowl-shaped mold, I don't think you will be able to find any other roughing strategy to come near it. Seriously, for a part that shape, due to the much deeper cut depth and higher feeds, I saw it cut 5 times faster or more than typical roughing strategies. For cores or complicated stuff, though, it is noticeably less good due to lots of repositioning and bad inefficiencies.

 

The good news for us is that VoluMill is going to be free of some of the technological challenges imposed by the TrueMill strategy, and we know how to avoid some potential pitfalls in our 3-axis roughing solution. I hope you'll consider checking it out when it's ready in '08.

[YoDoug®]

I finally had some free time this afternoon. This is a video of a 2d adaptive clearing toolpath from Cimco HSM. It looks just like the ones on the Surfcam website.

[esherbro]

There are some differences. As I mentioned above, Adaptive Clearing does really well on the outside of core parts (as you can see at the beginning of the video). Once it enters a channel, it seems to move to a trochoidal-like looping motion for most of the rest of the toolpath. TrueMill uses a similar motion to open up a new area, but then it goes around the opened area with longer racetrack-like cuts. If a part consists primarily of channels and constricted areas, I grant you, they will look quite similar. That's one of the reasons we pursued a different method for opening up channels for VoluMill, as I described above (going directly in, possibly with lighter axial depths of cut if the material or the stepover requirement warrants it). Thus far it's done very well and has performed noticeably faster than TrueMill.

[Glenn Bouman]

quote:

---

not sure your business odel is going to fly though.. a monthly charge that goes on forever is not an attractive proposition. I think most people would rather buy outright and pay a reasonable annual maintenance fee.

---

I agree, and I think your product would be much more successful if you make it available to dealers to demo and promote to end users.

 

esherbro, do you expect dealers to have to pay the monthly fee to demo, test and help sell your product?

[esherbro]

Glenn,

 

Dealers are a critical part of our business plan, and we are already partnering with dealers to help sell, promote, test, and support the product. Our dealer partners do not pay to demonstrate the product, we think our partnership agreement makes it well worth their while. Please contact me directly through our website if you're interested in learning more; we'd love to talk to you.

[YoDoug®]

esherbro, Have you done any testing of your tool paths in hard tool steel. That's where i see a problem with taking smaller axial depths to open a channel. If i am going to mill hard tool steel at small depths i would use high feed cutter geometry, for deep axial (peel milling) i use a different cutter. trying to do both with the same cutter is not a good idea. Also, spindle speed has a great affect on the ability to mill hard steel and small depths.

 

One other thing to note. We paid less money for our 1 network license of Cimco-HSM + 1 year maintenance than your cost for 1 a year 3-d subscription. The Cimco also includes many great high speed finishing passes also.

[Glenn Bouman]

quote:

---

Dealers are a critical part of our business plan

---

Since your software requires an internet connection to function it is impossible to demo on-site and for the majority of propective customers to use.

[esherbro]

quote:

---

Since your software requires an internet connection to function it is impossible to demo on-site and for the majority of propective customers to use.

---

There are machine shops without an internet connection still, yes, but a majority? That's certainly not the case around here, is it where you are located? Shops I have visited around here have their own websites, and email is critical to their business. Many of them rely on email not just for business communication but also to receive part data from customers so they can machine it.

 

As far as being impossible to demo, all a dealer needs is a laptop and an aircard that plugs into the PC-card on the laptop and accesses broadband cellular. It's cheap and means they don't have to plug into someone's network. When I was at Surfware all of our sales team had access to these cards when they were on the road so they could stay in touch with the central office anyway. This is very common nowadays.

[Mic]

Hi esherbro

 

Now I've tried your new interactive toolpath generator on your updated website. Very nice feature by the way.

 

First issue. Would it be possible for you to also upload dxf-files of the 3 parts? That way people has a change for trying the part in their own cam-system without having to use the 15 days trial period for a simple test.

 

Second issue. After having run a simulation of the toolpaths from the interactive site it stands clear that this is a very fast and efficient way to machine soft material like aluminium. But you can forget this approach for hard material like inconel and hardened toolsteel. The cutters used for material like these normally has a lot of teeth's ( 6+ ) and therefore a very small chippocket. This means that the d.o.c. for the opening cut of slots has to be very small not to overload tool. This will drastically increase the cycle time compared to truemill's trochoide motion for opening new area's.

[cadcam]

I know the Dealer that I work with the boss will not buy these cards so this make it not possiable. I do suggest a better way for dealers, as us dealers are going to help make most of your sales for you on most softwares.Of course this is your option as it is your software. But i have not even looked at till there is a way to show the customers and my students.

 

JM2C

[Guest]

quote:

---

Shops I have visited around here have their own websites, and email is critical to their business. Many of them rely on email not just for business communication but also to receive part data from customers so they can machine it.

---

While many shop do have all of the above mentioned, I am aware of a GREAT many machine shops that do NOT allow access to the people on the floor, it is tightly controlled and not everyone enjoys access.

 

Without some way for the dealers to be able to present this on-site without a connection, pushing it will likely not happen in a large way.

[crazy^millman]

esherbro,

 

Well I truly see a big gap in the reality of what you are after and what is going to work in the real world. What you see as ideal is going to limit what is going to be really out there for you to have the availability of the clients you think you will. I really hope you get the backing you are looking for. I see you painting yourself in a corner and test are limited to Aluminum. Address this market and go after it and might get what you need to sustain the business model you have decided to go after.

 

May seem like this is a slanted take on your approach, but your cost just doesn't justify the product you are trying to push. You are asking more for your product that is limited to your terms than what most pay for maintenance. I seem confidential issue's with parts and products where the product is not limited to in house processing will be a problem here as well. Many of my customers past and present do not allow or will be happy with the idea of off site processing thus losing control of security.

 

It has the approach of a good product and yes there is a need. I just think you would do better going after CNC directly verse thinking you are going to get what you will for the mass following of people willing to go off site for processing.

 

The last point is what happens if you go out of business tomorrow?? Where does that leave your customer with 50 to 100 files processed with your product that needs changes or tweaks like different tool, newer machine, newer geometry, or just plain old emergency and use what you got at the time. You leave them in a very bad place and you made your money for 1 or 2 years like you need to so you could move on like you have done like leaving Surfcam. Where do they stand if your guys developed it? Now they are stuck and so will your customers since you own it and we are just renting it to make you money for your next venture. Now if you are willing to put a liability clause that is insured in the case you do go out of business and my company could recoup tens of thousands of dollars in lost time and profit then it might be more attractive, but any bean counter that is worth their salt is not going to like the idea of opening up their company to such loses and liability without owning the product that is suppose to help make them money. Not possible hurt them in the long run like the business model you are offering does.

 

Again good luck, but I as a decision maker and possible user of such product see it as too much of a risk to think we will not go after it. Offer it as a stand alone wit ha yearly maintenance as a reasonable price we might talk, but Cimco HSM is at your price range and has a proven track record.

[esherbro]

Thanks again for the feedback. We really are listening, and appreciate what you are all saying. A few specific comments:

 

First, to Mic, an answer to your questions:

 

1) Done. If you go to our interactive demo page, you'll find hyperlinks by the radio buttons that will allow you download DXF versions of each part. I chose DXF because I figured it's the "most importable" format. Thanks for the suggestion.

 

2) We're still doing our testing on hard metals, so I don't yet have a definitive response for you yet. However, I will just note that if you are machining a slot in hard metal, there is a tipping point where machining time is less with a series of full radial/light axial depth of cuts versus a peel-milling/trochoidal light radial/full axial style of cut. What I mean is, if you make the slot long enough, the full radial cut will have a shorter cycle time, even with many axial depths of cut and even if you have to slow down the feedrate in the slot somewhat. This isn't just because of the longer path length and the much greater percentage of time the tool is in the air; in my experience, a peel milling approach can be even slower than expected if the machine's acceleration is too limited. The flip side of this is that as you decrease the length of the slot, at some point short slots will be faster with peel-milling.

 

Your point is well taken, and when we have more information we will definitely share it. We're keeping an open mind, and will adjust our approach if necessary based on the machining results. I do not believe we are inherently limited to aluminum, and if we need to adjust our toolpath to work better in hard metal conditions, we will. One of the really nice things about the client/server approach is that if we do find ways to improve the toolpath, we can deliver the benefits to all users immediately by upgrading our servers, and no customer has to upgrade to take advantage of the improvements.

 

Secondly, to Cadcam, JParis, and Crazy Millman, I appreciate what you're saying about this delivery model affecting both dealers and customers. You've all made good points and we are seriously considering your comments to see what we might be able to do to make things easier and more attractive for everyone. Nevertheless, based on our testing, we think the service will lead to reductions in machining time and extensions of tool life greater than the cost of the service within a few hours of machining. Ultimately, we believe those benefits and others still to come will drive the adoption of the techology.

 

Thanks again to everyone for the comments.

[esherbro]

Some additional responses to Crazy Millman's points:

 

1) I can't go into detail here, but there are options for customers of a certain size who have security concerns which would allow them to control their data as they see fit. However, some customers who would not want to send out their full designs might have no problem sending out simple individual 2-D pocket geometry that gives no indication of the full part they are actually making. We have talked to a few facilities with high levels of security who have had no problem with this, and they are happy with our heavy encryption and guarantees that their data will never be saved by us.

 

2) In practice, going out of business is a risk you run with any software you purchase, and it's a risk your software providers run with providers of technology they license. Not only do you lose support, training, upgrades, etc. for the product, at some point you will lose the ability to do data exchange with other products, and possibly it will not work at all when you have to do an OS upgrade. With a service business, one of two things usually happens: either it is generating no revenue, in which case it stops, or it is generating some possibly small amount of revenue, and some other company purchases the right to keep it running; because it is generating revenue, there is a value to it. If the technology has enough value to customers that they need to use it to generate toolpaths, the service will exist in some form. If it does not have enough value, the customers will stop paying for it and choose other solutions. Ultimately, I suspect it would be far worse to buy an expensive CAM system from a company that goes out of business six months later.

[crazy^millman]

Thank you for your answers and honest understanding that I as well as others have done this a day or two. I honestly think you have a good product and wish you the best at this time there is enough capabilities in Mastercam and I have other tricks that make it do what we need and get the job done in timely fashion. We will be watching to see how you grow and keep things going.

 

Again good luck and hope to see you around the forum.

[babolino]

hello all,

 

I think as long it makes "sharp corner moves" its wothless for me:

 

 

maybe I´m doin something wrong?

[MultiAxGod]

Don't have as much time to comment as I would like because I have to get some work done!!! LOL

 

We tried VoluMill here on Proprietary steel similar to 4340 @ 45R on a Makino HMC. The cut was a periphery cut going in and out of material thickness. Volumill saved time from 2:45 min to 2:30 min per revolution around the part and from 4:30 to 3:15. We are attempting to not only save time, but more so of insert life, which are currently changed after every part (26 inserts).The feedrate does change and is not constant.

HFM would not do the cut period and never got a response from CNC.

Sorry Evan, we are also trying CIMCO because of the Internet connection issue, but your software and the algorithms do work well. VoluMill was also very responsive to our needs and communications and resolutions were typically in minutes.

If I can get more time I will add more information as to what we did and how it all worked.

 

 

[MultiAxGod]

Just a quick update.

We cannot use CIMCO or Mcam HFM because neither support slot mills or undercuts. VoluMill did and supported the centerline of the cutter outside the boundary.

Thanks Evan.