CnC head software ?

Post by **SchmidtMotorWorks** » Fri Jun 10, 2005 10:36 am

Most good places for rapid protoyping have 3d-scanners, and will suplly you with an editable, 3D-CAD file in either proeng. or catia format.

That depends on what you mean by editable.

Yes you can fit surfaces to scanned points and you can "edit" thier shape by dragging the control verticies but the results are unlikely to be satisfactory.

For example in the case presented earlier of raising the roof of the port. If you try to do that by selecting a region of poles that cover the top of the port and translate them up you have a choice, either to move the poles along the axis of the valve or along the axis of the intake port face. Either choice makes unintended changes in shape to other areas. If you move it along the valve axis you will have a problem near the port opeming, if you move it along the port opening face the valve guide boss shape will lose concentricity to the valve. In both methods you will have some weird blending in the transition from the bowl walls to the top of the port particulalry where the radius of curvature is is large. This is because the set of poles you move will usually need to be a rectangular set of rows and columns to keep the surface smooth in the middle but if that rectangular selection includes the top of the port and the adjacent radii at the top left and right sides of the port the rectangle will cut somewhere across the much larger radius at the bowl. What ever you do there, you will be installing some kind of S shaped transition there. You can then go back and move single control verticies one at a time and try to blend it out but this is where you begin wishing you had a parametric model.

With parametric models, you can edit dimensions while retaining the design intent. Scanned models have no design intent or parametric features.

cboggs · Post by **cboggs** » Fri Jun 10, 2005 12:46 pm

One thing brought up by Jon, .. is the cost of this software.

I've been told that Pro-E is around $30K a year !! ???
is that true??

Mastercam & Surfcam are $15 to $30K with a minimal yearly
charge, ..

Donovin, .. the Fryer 5 axis machine looks nice, .. and seems like
it might be reasonable for costs, .. thanks.

The big key for me, .. I'm a small custom shop, .. not huge runs,..
so I want to keep the costs down so I don't get killed by overhead.
I've heard a few stories if guys buying $300K worth of CnC and not
making the nut, ..

So even if it's a used 4 axis machine, that I have to hand finish ports, that's just fine, ..

OK, so back on topic, .. Jon, .. we should talk in more detail, ..
you speak of the "big three" but as I brought up there are some costs
involved, .. what are the trade offs to using Surfcam / Mastercam
VS, the "big three" ??

As far as scanning, .. touch probe scanning in the spindle, .. seems
to be common on "low end" CnC head work, .. anyone know
about this process?? Many shops charge $1K - $3K to scan a head, ..
I assume the cost has to do with the file prep?

Good thread, ..

Curtis

Post by **SchmidtMotorWorks** » Fri Jun 10, 2005 1:09 pm

I've been told that Pro-E is around $30K a year !! ???
is that true??

Good news, you can get set up in any of the big three for 25K for modeling and CAM. Most have monthly maintance about a couple of hundred a month (I don't work in sales so I don't know much about prices).

UGNX has vastly superior surfacing and CAM than Pro E, that's why Pro E isn't used much for auto body design but it is used for mechanical design. CATIA has reputation for good surfacing but I haven't heard much about CAM.

Don't underestimate the difficulty of modeling complex surfaces like ports. They are no less dificult than modeling auto bodies and things like golf club heads (suprisingly difficult). Nobody uses CAM software or mid-range stuff for that work for good reason.

So even if it's a used 4 axis machine, that I have to hand finish ports, that's just fine, ..

I think that is a good decision, you might even use a 3 axis machine with some fixed angle fixtures to get started. I have seen some 5 axis set-ups that really do a lot of movement to remove a little metal that could be really simplied if they used a more capable CAM software.

what are the trade offs to using Surfcam / Mastercam
VS, the "big three" ??

The main things are

#1 You absolutely must have parametrics so that you can adjust dimensions of your design and all the surfaces will still fit together instead of needing to recreate new surfaces.

#2 You need a set of surface tools that has the abilty to model many types of surfaces with different controls. For example NX has somewhere in the range of 10 basic surface types with sub-types and options running into the hundreds and I sometimes ask for additional control options.

Most of the CAM surfacing software don't have capabilty to define surface continuity (the abilty to have tangent or curvature continuous relationship) .

As far as scanning, I have also done lots of indicator "scanning" it is time consuming but it ussually works out OK in the end and sometimes I find things that I wouldn't have noticed otherwise.

learner · Post by **learner** » Fri Jun 10, 2005 1:19 pm

Without stealing the thread i have one question for Jon. Do you do investment castings?

Thanks

Post by **SchmidtMotorWorks** » Fri Jun 10, 2005 1:30 pm

Do you do investment castings?

Yes, I just finished an investment casting mold for Stewart Van Dyne for a valve cover for the LS1 where additional clearance is needed for aftermarket shaft rocker systems.

I also did a water pump impeller.

Probably best to start a new thread about investment castings if you want more info on that subject.

One thing about investment casting, I find the accuracy claims are wildly exagurated. One recent project was predicted to shink 0.018" per inch and actually shrunk 0.012". That meas on a 20 inch part you have a peice of junk on your hands, start over.

Post by **SchmidtMotorWorks** » Fri Jun 10, 2005 1:34 pm

You know, I think to explain this I should make a series of images explaining the steps to modeling a port parametrically and then adjusting it.

I'm going to Ohio this weekand until Tuesday so I can start it after that if there is interest in how to model ports.

Anyone have advice on Springboro?

learner · Post by **learner** » Fri Jun 10, 2005 1:39 pm

Jon i will send you an email. I'm interested in the modeling process.

shawn · Post by **shawn** » Fri Jun 10, 2005 4:43 pm

I spent a few years doing cnc machining and have always wondered why you couldn't use a 3-4 axis machine to at least rough in a port. I'm sure Curtis will agree, moving the large amount of metal required on some of the ports is extemely time consuming, and if you have a realatively inexpensive 3 axis machine that would rough those in for you it would save a ton of time. Most of the people that i have talked to in the past have always poo pooed the idea of using anything but a true 5 axis machine.But for the rest of use,who could make better use of time, don't have a ton of money to spend,as well as use the 3 axis for other small projects,it would be a good investment. If the software available would do this, you could invest in it and upgrade to a more "complete" machine later. Is this something that sounds feasible? Or am i just looking for something that isn't really atainable?
thanks,
shawn

Post by **SchmidtMotorWorks** » Fri Jun 10, 2005 6:13 pm

Two years ago at WESTEC (a big machine show in LA) HAAS or FADAL had a 5 axis machine running a fuel head in it going through the motions on a cut head. I'm guessing it was John Forces head.

I had just finished my fuel head model so I was really interested to look for any unusual features in their head. I probably stood there for three hours to see all sides of the head.

What was most amuzing was they were using 5-axis motion where it was complelty unnessary in places like the chambers etc. The way the tilting fixture worked the cutting point might have moved 10 inches for every 0.1 inch that the cutter moved along the head. This invites innacuarracy and slow machining.

It was interesting to hear the comments of the people stopping to see the machine running. Some people were really excited by all the motion and just liked to see anything related to Hemis.
The 5+ axis aerospace CAM programmers moslty just cracked jokes about how inneffient the the methods of cutting were.
Just goes to show, software and equipment aren't enough.

I think about 6 fixed set-ups could machine the vast majority of most ports. Probably much faster and more accuratly and safely than 5 axis simultaneous motion.

If you have the models in CAD you can determine this before buying any equipment, no reason to guess on this matter.

Harbinger · Post by **Harbinger** » Fri Jun 10, 2005 7:00 pm

Interesting thread, but I'm wondering if things aren't already way off track?

Curtis,
I understand that you have already developed ports by hand and you'd like to have those ports duplicated, create an NC program in a CAM system amd have a cnc machine reproduce your work?

While I agree, being a manufacturing engineer, that the process of creating a port shape from scratch is exciting... is it really something YOU need to do?

Do you want to do the work in house, make that investment in software, training and machine tools, or would you rather send the master port for digitizing, programming and machining? If the later, then I can put you in touch with a number of guys who do just that.

I am a CAM programmer and have been doing this for a number of years now in the injection mold, aerospace and most recently, PIR motion sensing lens arrays. I've worked with UG, Solidworks, ProE and a number of other design packages. Probably worked intimately with a dozen CAM packages. So I consider myself "up" on the industry.

If your company's mode of operation is in developing master ports (by hand), digitizing, CAM programming, 5-axis machining.... then I see very little need for UG, Catia or ProE. They have their place, they are all three very nice software packages, but I don't see them being a necessity in your situation.

I speak with some experience, either in programming this type of work or in working with people doing what it is you'd like to do. Machine ports. If I were looking to do this, I'd have an outside source digitize, then use Raindrop Geomagic to create the NURBS surfaces, then use Mastercam or SurfCam to create the NC code. I would not lock myself in with a dedicated 5-axis machining center but would instead use a 3 axis vertical machining center and a trunnion to get the work done. You will also have far fewer surface violation problems and much more efficient cutting speeds if you will program with 4/5th axis positioning only, rather than 5-ax simultaneous. You will also want a control which is NURBS capable. That rules out many of your less expensive machines. FWIW, I would not buy a Fryer.

If there's anything I can do to help, please let me know.

Harbinger · Post by **Harbinger** » Fri Jun 10, 2005 7:32 pm

shawn wrote:I spent a few years doing cnc machining and have always wondered why you couldn't use a 3-4 axis machine to at least rough in a port. I'm sure Curtis will agree, moving the large amount of metal required on some of the ports is extemely time consuming, and if you have a realatively inexpensive 3 axis machine that would rough those in for you it would save a ton of time. Most of the people that i have talked to in the past have always poo pooed the idea of using anything but a true 5 axis machine.But for the rest of use,who could make better use of time, don't have a ton of money to spend,as well as use the 3 axis for other small projects,it would be a good investment. If the software available would do this, you could invest in it and upgrade to a more "complete" machine later. Is this something that sounds feasible? Or am i just looking for something that isn't really atainable?
thanks,
shawn

Shawn,
This is a feasible process. Of course a 3-axis mill can only complete so much of the port on a given trajectory angle but that should save you a good deal of grinding time. Look to 200+ degree ball shaped burrs in long length to get as much reach as possible. OSG Sossner makes a very nice shrik-fit system that works well for this type of cutting with very minimal TIR.

Post by **SchmidtMotorWorks** » Fri Jun 10, 2005 7:37 pm

If your company's mode of operation is in developing master ports (by hand), digitizing, CAM programming, 5-axis machining.... then I see very little need for UG, Catia or ProE.

I agree, if you only want to duplicate ports you could do it with the non parametric, non integrated software. I am suggesting that he consider a different approach. I think that the scan and cut based method leaves a lot of opportunity for improvement on the table and no efficient way to make changes or series of experiments that you could have with a parametric port. With all the porting people on the market this could provide him with a significant differentiator from the competition.

Gaining these skills also moves one closer to being able to design a head and tooling with the best methods and fewest dissapointments.

Maybe someone can post some scanned ports that were surfaced in any RE system with both the points and surfaces? Then I will make a parametric model to compare and we can see the difference.

cboggs · Post by **cboggs** » Fri Jun 10, 2005 10:00 pm

Jon,

#1 You absolutely must have parametrics so that you can adjust dimensions of your design and all the surfaces will still fit together instead of needing to recreate new surfaces.

Doesn't GeoMagic let you do this?

Harbinger,

You bring up several good points.

first, sending stuff out to get scanned & CnC ported, like I do now, ..
has several draw backs, the big one is costs, ..

To scan and prep the files most people want from $1K to $3K, ..
then $100+ an hour machine time to cut, .. I can't resell the work and
make a profit.

If I'm cutting 20 heads, yes it's worth it, .. if I'm doing two sets, ..
it's no where near worth the investment.

I'm a custom shop, .. doing small runs of stuff and need to do
the CnC in house for that reason. Fast turn around is another, ..
and keeping some designs all "in-house"

I'm with Shawn that what I really want is a simple solution to
increase my productivity, .. to CnC bulk material and hand finish
the heads.

So from that stand point, .. using Geomagic & Surfcam, .. and a 3 axis machine
with a fixture or even a 4 axis machine and position cutting sounds
like a very good, .. and the "simplest" plan.

My question is this, .. Jon, .. Harbinger, .. couldn't both work flows be
used depending on the need? Geomagic & surfcam for the hand port
& copy work, .. and Pro-E for the deeper development work?

Now about the scanning part, .. can I digitize in the spindle with a
touch probe?? Fero arm, .. ???

Oh, .. Harbinger, .. what's your first name? pet peeve of mine, ..
I'd like to use your name to properly address you if you don't mind.

Curtis

Harbinger · Post by **Harbinger** » Fri Jun 10, 2005 10:11 pm

SchmidtMotorWorks wrote: I agree, if you only want to duplicate ports you could do it with the non parametric, non integrated software. I am suggesting that he consider a different approach. I think that the scan and cut based method leaves a lot of opportunity for improvement on the table and no efficient way to make changes or series of experiments that you could have with a parametric port. With all the porting people on the market this could provide him with a significant differentiator from the competition.

I have to disagree.

If a highly successful port has already been developed through countless hours of testing and trying ^10, why start from scratch with a parametric model? Doing it just because you can doesn't make good business sense to me.

Slightly off our main topic, but I would hate to spend the time and money developing an intake port through parametric modeling or whatever other means available that performs worse than an inexpensive and readily available Edelbrock Super Victor. Now consider the development time already in the Edelbrock intake design. Why not try and improve on that instead?

How does this differentiate him from the competition?
I bought a set of Hutter ported 18 degree heads last year from Weld Tech. I have no idea what revision number they were.

In the end, a customer gets a cylinder head. Will the customer really feel that he's getting something better just because Curtis abandoned his proven port and developed a parametric model to cut a new one from? Or that he used 30 revisions to get there? Does the cutomer even know what "parametric" means? Does he care?

I don't know about you but if I were going to buy a cylinder head from a porter who has developed a proven design, I don't want that new "parametrically designed" port. I came to him probably due to his success with the old one and I'm hoping he has tweaked it a little.

edit: Let me answer your questions tomorrow. I've been on the phone for the last hour or so with this response ready to go.

Thanx.
ChuckM

Post by **SchmidtMotorWorks** » Fri Jun 10, 2005 10:38 pm

Chuck,

You are ignoring a key point, when you model a a port parametrically with the scanned port as a reference model you will find shapes in the hand formed port that you didn't know were there. The difference between judging the shape of something looking down a hole and examining it with all the curvature analysis software that good CAD systems have is massive.

Maybe those odd shapes that you don't know about actually help but maybe they don't and that is the benefit of making clean models you can easilty make one wothout the odd shape you find or try making it bigger by an exact amount and test the result.

Like I said before, even the simple fuel heads that I reverse engineered that were moslty CNCed had different lumps in every port and I will bet you anything, they weren't intentional.

Having a parametric model provides a baseline for experiments that you cannot achieve with a die grinder.

If you used your logic on other fields that rely on defining the best shapes like, airplanes, propellers, impellers, boat hulls, car bodies etc etc. you could not compete in modern times. The same is true of ports, when I worked at Honda, there wasn't one part of the heads that were touched by a die grinder.