Need2 define a Cutter, with a large spherical radius, ALSO be able to drive Barrels mills with MAFC

Hi Friends,

We, and I mean you, and I and all of us, Need to define a Cutter, with a large spherical radius, and......also be able to drive Barrels mills with Multi-axis Flank

We have a requirement to machine a part with a 1.25 Dia cutter with a  5 inch spherical radiuson the bottom. But there is no method to define such a cutter as it truly is. People do use workarounds.  Lie and then use a user rep, ... but that requires containment sketches, and messes up automation for shop docs, and you say 10 inch dia Ball, when it is really a 1.25

What a cutter like this is good for is for machining parts with a small amount of curvature. Everyone I know has used these tool for years....This is very efficient, and reduces the amount of hand grinding on parts when done.

This could be both 3 and 5 axis. You can imagine that the same result of finish would be gained by either 3 or 5-axis… and the reason for wanting 5-axis would be to tilt a little to no cutter with the area of the tool near the center line, that is usually going very slow constant surface speed, and also… if you need to tile of he floor is at a steep angle.

This is a very important function, as this is a STANDARD tool for the aerospace industry.

We define this kind of tool in NCL by saying I have a 6 inch diameter 3 radius ball with .0658 height. The height makes the tool what we call a disc. Note in NCL the side .125 rad not defined in this method

This tool is also definable in UG-NX.

++++++++++++

Another topic that is related is to be also be able to drive Barrels mills with Multi-axis Flank. I like the new tool definition. I know sometimes DS will give us a new function... like the new Barrel with limited usability, and request Feedback.

My feedback is the next MO I would like to see barrels used on is MAFC.

I have Vetted this enhancements with a few friends, and all agree this is important functionality, so I hope DS can plan to put some people on it.

In the mean time, I hope you COE members, can help define the requirements in more detail.

Best Regards

Dave

Hi Dave,

If DS folks ever decide to put this type of tool then I would like to see a few things. Basically my idea is to define the tool with the minimum user interaction. I know UG allows this type of tool but their interface is very painful since you need a calculator to fill the parameters. I hope DS would do it better.

Attached is image of this cutter where I defined required parameters including some for the shank and overall length. And this goes for all the type of cutters and holders.

For example: lf you need this cutter with tip-radius of .500 and 1.25-diameter at the Corner-height (intersection of tip-radius and the flank of the cutter) say .250. All you need to enter is these few parameters along with any lead-angle/taper-angle. And all other 4 parameters for the center points of the tip and the corner radii are calculated automatically.

Thanks to the Sketcher in Catia. Because it helped me to determine the minimum number of the required parameters for the input. And there must be a Range settings for the lead and taper angles just in case if user is not careful. These calculations and validations are required for such tool-types especially for T-slotter, Barrel-mill, Conical-mill, Boring-tool including Holders(Tool Assemblies) as well.

P.S. These ideas/enhancements are brought up by V5 customers. I hope that DS takes an ethical approach and would add such functionality for the V5 customers. And I have already sent this file to the developers at DS.

Samarinder

Hi Samarinder,

I like you comments. So people know, I vetted this enhancment request with 12 power users, and I got overwhelming responces that

 

1. We need the Spherical radius cutter

2. The barrel cutter needs to be usable for MAFC

3. I also got descriptions for other special cutters, like the one Samarinder just posted.

4. All users EXPECT Catia to eventually be able to handle ALL tool descriptions, that programmers are REQUIRED to make toolpath for.  One user made this point by saying he used NCL, because it can to 100% of what is required, not 95%

 

I expect DS to add these tool, and what we as users and COE members need to do is say what the requirements you have are.

 

This is important, so DS works on the most important implementations first.... since the can not waive a want, and give it all at once.

So please follow Samarinders lead and state your requirements.

 

Dave

Since we are talking special tools we also need another:

 

MAFC is required for T-Cutters.

 

Dave

Whatever you guys decide, I'm with you 100% on this topic. I asked for this cutter definition years ago, also pointing out that APT could do it decades ago creating a "ring" cutter a Dave described. I have driven this type of cutter many times in CATIA but the workaround is painful, tricky sometimes, and always time consuming. For certain parts the result at the machine is far worth the effort.

Anyhow, one can dream....as long as there are workarounds, however painful, these things don't usually become a priority.

But this is such a common cutter, I really think it should have been a priority long ago. I've never used a barrel cutter and don't even know where one can purchase one. I'd gladly trade it for this tool description if it could be used in any mo type. I can't remember ever once needing to use a barrel cutter to multi-axis sweep!

Whatever you guys decide, I'm with you 100% on this topic. I asked for this cutter definition years ago, also pointing out that APT could do it decades ago creating a "ring" cutter a Dave described. I have driven this type of cutter many times in CATIA but the workaround is painful, tricky sometimes, and always time consuming. For certain parts the result at the machine is far worth the effort.

Anyhow, one can dream....as long as there are workarounds, however painful, these things don't usually become a priority.

But this is such a common cutter, I really think it should have been a priority long ago. I've never used a barrel cutter and don't even know where one can purchase one. I'd gladly trade it for this tool description if it could be used in any mo type. I can't remember ever once needing to use a barrel cutter to multi-axis sweep!

Whatever you guys decide, I'm with you 100% on this topic. I asked for this cutter definition years ago, also pointing out that APT could do it decades ago creating a "ring" cutter a Dave described. I have driven this type of cutter many times in CATIA but the workaround is painful, tricky sometimes, and always time consuming. For certain parts the result at the machine is far worth the effort.

Anyhow, one can dream....as long as there are workarounds, however painful, these things don't usually become a priority.

But this is such a common cutter, I really think it should have been a priority long ago. I've never used a barrel cutter and don't even know where one can purchase one. I'd gladly trade it for this tool description if it could be used in any mo type. I can't remember ever once needing to use a barrel cutter to multi-axis sweep!

UG did whip everybody's butt with their cutter definition.  And that was about 25 years ago

I too hope to see some of these drivable cutter definitions in V5.

In Reply to Bryan Carpio Felsher:

Whatever you guys decide, I'm with you 100% on this topic. I asked for this cutter definition years ago, also pointing out that APT could do it decades ago creating a "ring" cutter a Dave described. I have driven this type of cutter many times in CATIA but the workaround is painful, tricky sometimes, and always time consuming. For certain parts the result at the machine is far worth the effort.

Anyhow, one can dream....as long as there are workarounds, however painful, these things don't usually become a priority.

But this is such a common cutter, I really think it should have been a priority long ago. I've never used a barrel cutter and don't even know where one can purchase one. I'd gladly trade it for this tool description if it could be used in any mo type. I can't remember ever once needing to use a barrel cutter to multi-axis sweep!

 

 

Hi Bryan,

100%... I like it. Thanks for the support.

Most big companies grind there own cutter like this, in house. We have 5 CNC carbide grinders, along with our clasic monosets, and other cutter grinders.

I used these all the time in NCL.  I used the barrels, for cutting slight curvature on inside walls that are true offsets, and not ruled surfaces.

There was a word you used on another topic, and I had to look it up.... intrinsic.  Yes, these cutters should be intrinsic withing Catia.

Best Regards

Dave

In Reply to Roger Bombassei:

UG did whip everybody's butt with their cutter definition.  And that was about 25 years ago

I too hope to see some of these drivable cutter definitions in V5.

 

Hi Roger,

I hope so also. Thanks

Dave

Dave,

The first priority on my tool wish list would be the large radius bottom tool, hopefully with corner radii included. I don't think I've programmed for a shop anywhere that does not use this style of cutter. We really need to impress upon the developers just how common and widespread the use of this tool is.

A lot of people may be unfamiliar with the barrel cutter, so I'll have to do a history lesson.

The barrel cutter came from Douglas Aircraft. Because of their resident genius, Paul Mills, Douglas was the first aircraft company that had mathematically defined loft surfaces in a computer format. They also had an extended APT add on program called DAC-ARLEM that could take advantage of these mesh defined surfaces.

The barrel cutter was developed to efficiently cut inside of a concave surface. By specifying different cutter contact height for the barrel cutter, the concave surface could be cut in just a couple of passes. What would take 50 or more passes to keller with a ball nose could be done in 3 or 4 passes with a barrel cutter.

 Paul Mills later developed NCL, so that's why NCL has barrel cutters. McDonnell Douglas's McAuto division at one point owned Unigraphics. That is why Unigraphics has a 10 parameter cutter definition.

Those that programmed outside of the Douglas sphere of influence may never have used a barrel cutter. Boeing had their B-Surf routines, but compared to what Douglas had, it was quite lame in comparison.

 

When Dassault licensed NCL's tool path strategies, I would have thought that the 10 parameter cutter statement would have come along with it. And then when a barrel cutter definition finally was added, I would of thought that the first and most logical operation to use it in would have been MAFC. MACF is where the barrel cutter should be deployed, it's useless anywhere else.

          

Randy Hitzeman

Hi Randy,

Very well said.

 

Now, a question for you and everyone else. On the spherical bottom tool

 

1 Would you if given the choice to have no radius first, and then get the radius a few service packs afert.... would you take it? I would.

2. Which MO's would you like to see it used on. All is an ok answer, but I think priorities help.

 

thanks in advance

 

Dave

Dave,

Agreed. I will take what I can get for now on the spherical bottom radiused cutter. The corner radiuses later would be frosting on the cake. 

 

Randy Hitzeman

Bryan is in France and asked me to post this for him.

 

When I program these tools, I almost never actually drive from the corner radius. I would like to see it available for MAFC 1st.

Thanks Randy for the excellent explanation of the barrel tool. After your explanation, it makes sense. What makes no sense at all is why the tool is only used in CATIA for multi axis sweeping. I can't think of when that would be useful, especially since that MO drives the bottom of the tool only.

Best,
Bryan Felsher
True Precision
Ph: (310) 750-6761
Cell: (310) 756-4534
Fax: (310) 706-6378
www.trueprecisioncnc.com
[login to unmask email]

 

Here’s a doc that describes UG milling tool definitions -

http://www.steptools.com/library/stepnc/2010_nist/presentations/MILLING_TOOL_PARAMETERS_DOCUMENTATION.DOC

edit- not sure why I'm getting so much space and I'll try uploading the doc since the link doesn't work

Roger,

Great document. It's a concise explanation of a 10 parameter cutter definition.

 

Randy Hitzeman

In Reply to Randy Hitzeman:

The barrel cutter came from Douglas Aircraft. Because of their resident genius, Paul Mills, Douglas was the first aircraft company that had mathematically defined loft surfaces in a computer format. They also had an extended APT add on program called DAC-ARLEM that could take advantage of these mesh defined surfaces.

         

 

I have Copy #129 of the DAC-ARLEM user's guide on my book shelf along with the Convair (Fort Worth) NC programming manual dated 1957.  The F-111 was lofted with APT polyconic surfaces but I can't dispute your claim of DAC being first.  We were doing it in the mid 60's I think.  We have done NC programming in this building for 55 years.

Our residant geniousus had their own cool APT extension called WOFSET.  This allowed the geometry to be driven with a zero diameter cutter normal to the surface (easyest to compute) and then transforming the output to the tool tip.  Made the APT cutter shape irrelevant but check surfaces a guessing game at best. 

Jim  

If I'm not mistaken, McDonnel Douglas created UG.  And they probably used the DAC 10 parameter cutter.  Just guessing...

In Reply to Randy Hitzeman:

Roger,

Great document. It's a concise explanation of a 10 parameter cutter definition.

 

Randy Hitzeman

Roger,

Unigraphics was created bu United Computing in Torrance CA.

United Computing was known for UNIAPT, the 1st APT system to run on a mini-computer.

United Computing licensed one of the granddaddy's of CAD called ADAM. Automated Drafting And Machining.

From this they created Unigraphics.

McDonnell Douglas bought it in 1974, and sold it in 1991 to EDS.  

Randy Hitzeman

I worked at McDonnel Douglas in Torrance in the early 80s and I knew they owned UG then.

But they had a better system at the time called CAD E.  I used both of them.

I also worked for Automated Design Centers in 80s.  The guy that owned that company (John Wright)  was involved with creating UG.

I forgot that it was origanally created by the same people that created UCC APT.  I think UG came with UCC APT back then too.

Roger,

It was United Computing and UNIAPT. UCC APT was another APT system, but not the same.

John Wright was the founder of United Computing, and came to McDonnell Douglas when they bought Unigraphics.

Randy Hitzeman

lol, I'm so confused.

MDC APT, APT-AC 370, NCL, UNIAPT. UCC APT, 360 APT, DAC ARLEM

I think there's still an NCL programmer where I'm at now.

Speaking of DAC ARLEM, and Paul Mills, when I took my NCL fundimentals class in 1987, Paul Mills son was working for NCCS, and in the class.

The teacher as I said before was COE member John Gates

In Reply to Roger Bombassei:

lol, I'm so confused.

MDC APT, APT-AC 370, NCL, UNIAPT. UCC APT, 360 APT, DAC ARLEM

I think there's still an NCL programmer where I'm at now.

I have nothing but respect for the people that programmed in these systems, without Vericut... graphics, motion display, or the fixture........ just their imagination  of what in 3d the part looked like... and programming the back side with the 0,0,-1 tool axis, and the tracuting upside down.

 

Cheers.

Dave

It make you think how good the software is today, were you don't need to know how to compute a point on the UV of a cubic patch, or what a matrix is, or how to translate points thru a matrix manually.  Etc, tec, etc.

Any knuckle-head can make tool path today.  Back in the day we hand wrote the program code, had it punched into cards, sent to the mainframe lab, wait overnight, get the printout and cards back, fix the section 1 errors, repeat as needed, fix section 2 errors, repeat as needed, finally review the post output line by line, send the data to the flatbed plotter, review the plots, make corrections, repeat, send the final data to get a tape punched.

We were lucky to get a simple 3 axis job done in a week and 5 axis jobs took months.

And, we had to walk to work in the snow.

lol, I started programming with punch cards.  That was a long dragged out process.

We had to visualize everything.  Starting with blueprints to visualize the part.  There was no CAD model.

Then we visualized the machining.  There was no Vericut or tool path replay.

Not many people could do it then and there's not many that could do it now.

So, back to the original subject.

Dave, did you say that Dassault suggested that for a barrel you program with the bottom of the tool and tracut each point 90 degrees?

I love a challenge. :)

I remember when we used to have to program railtop radii with a ball the size of the cutter corner rad the tracut into place......  lol

Where else can you have this much fun and get paid

That was proposed with an exchange of emails with COE members and others. I thought it would be easier to program a 20 inch ball, and try to crop the motion to stay inside the radius of a 1.00 dia cutter.

But yes...... tracut 90 on a barrel... that would be fun to try.  Numbers dont lie. It would work.

But  the sweep MO is to limited. MAFC as stated is the MO of choice, for a Barrel.

Dave

I think we can all see that it's not too tough to make a spherical bottom cutter to work with the current CATIA

But the barrel would be a major pain

If you were following a ML contour your 90 degree rotation would be changing at every point.  I can't imagine anyone doing that.

While we are at it, I think it would be incredible if we could gain control of the 90 degree head.  Normal or tangent to double curved surfaces.

We want it all please

Hi Roger,

The 90 deg tracut, would apply for 3 axis, to fake in sperical tools using a Barrel. There is that old requirement to lie about the cutter....

 

As far as 90 heads, what "gain control" are you looking for? we can post any MO for 90 head, and simulate with "too expensive for some but not all" License for Maching builder, and Machine Simulation.  ... By the way, I hear some MB or MS is included in V6... not exactly sure so don't quote me.  Mark Chitjian, do you know about that?

Anyway, What control exactly are you looking for? You always have good suggestions.

I would like to be able to program and video replay a 90 degree head just like any other cutter.

I don't understand why it isn't common practice.  All of the angled head programming I have done was by creating geometry to drive at the center of the main spindle.  Not fun and too time consuming.

I know ICAM can be set up to do all of the translations but I've never worked anywhere that used it

I imagine ICAM can do the translations for programming a barrel shaped cutter using the bottom of the tool in CATIA

Maybe I'm asking too much but I prefer to do the work in CATIA without add ons or fancy post processors

I don't even use VB scripts

Hi Roger,

I could use a Barrel-mill in MAFC on my current project. I wonder who would be using it in MuliAxis Sweeping MO. If NCL can drive Barrel-mill for flank milling the walls then why not MAFC. I would like to say that whatever cutter/strategies were available in NCL 10 years ago must be supported by MAFC in V5. But then again if it wasn't done that time then no problem I can wait for it because I would like to see other most frequently used items first in MAFC such as

1. multiple axial depth levels same as Variable depths in roughing MO. You would be surprised to know that there is some other brand-x cam package does it in the 5-axis MOs for finishing the walls.

2. TLAXIS settings for check surfaces at start and stop. So users don't have to create extra planes, surfaces in the NCGeometry catpart.

3. local modification: more control for setting fixed tool-axis. Not just one global tlaxis for every drive surface. Local-mods needs local fixed tool-axis

4. variable corner smoothing in HSM. Not just one value everywhere. My idea is to use max and min values and then gradually decrease the value for every Radial pass by the amount of radial stepover. This is exactly what I do when creating custom geometry with my powercopies. This idea can be implemented in other MOs as well.

5. machining areas for MPs using MAFC and this is must have for every MO in Catia.

Anyway there is another thread where we listed lots of other items just for MAFC.

Regarding 90deg head: Icam does a pretty good job for 90deg head-attachments. I have programmed full 5-axis motion using 90deg heads and written an extensive set of macros in Icam especially for the FIDIA C20 control. I have been using Icam for over 2 years now and all I can say that it gives an absolute control on how to output the G-code period. But it is very expensive for small companies/contractors.

Another way of doing 90deg in Caita is TRACUT and then use a regular 3-axi or 5-axis post depending on the tool-motion. But tool-motion-replay needs MSG license for the head-attachments. I wish if it was part of AM2( advanced machinist/machining).

PS Thanks to Dave for giving me some tips on Icam 90deg head-toolchange-syntax which are not documented in the Icam manuals.

Samarinder

I LOVE these ideas!!!

P.S.  I drive T-slotters all the time in MAFC.  I just lie and use a regular endmill and a user rep.  Works for me, but yeah...don't see why it can't be done by default.

 

Again....ALL cutters should be available in ALL MO's.  All macro's should be available in ALL MO's as well.

 

Anyhow, hope we get this new tool description.  I've done it a bunch, but it is kind of tricky.  In MAFC, I'll use a 2" ball with a user rep and a NEGATIVE offset on drive surfaces.  It works well.

Bryan, are you  saying you use a ball to create motion to drive a barrel without translating?  Now that you mention it, I can see how that would work.

When I'm cutting a pocket in a typical aerospace door, the floor might be a
1000 inch radius with canted walls. Using a 1.00 dia tool with a 2" radius
on the bottom and .125 corner radii lets me finish the floor and floor
fillets with a pretty nice floor finish. I'll typically rough, then finish
the walls with whatever tool will allow to finish the corner radii- say a
.500 with .03R and finish tangent to the .125 floor fillets.

Then, I need to finish the floor, so that's when I'll use the special tool.
I might sweep back and forth on the floors using a sweeping MO, then finish
the walls (to clean up the floor fillets) using MAFC. What I do is use a 2"
dia. ball endmill and a user rep. I'll "lie" to it and enter a -.500 offset
on drive surfaces. Basically the MO is driving the center of the 2" dia
dummy ball endmill.

It's worked really well for me.

As far as finishing walls with a barrel type tool- basically "kellering" the
walls with the side of a barrel tool....well, in all honesty, I've never
tried doing that or been asked to do this. The only way I would even
consider doing this in Catia is if the wall to be finished was wide open and
I could use a fixed tool axis. Then, I would just tracut it. Other than
that, there's no way to do this in Catia. You would have to have a post
processor capable of doing the translation, similar to the way
post-processors control 90 degree heads.

I have programmed lots of 90 degree heads in Catia, even doing some pretty
complex multi-axis motion with 90 degree heads. I just program them like
any other tool, and my AZPost processor does all the work. I simply choose
the correct LOADTL sequence, containing the neccesary statements to tell the
post that it's a 90 degree head, and it does all the rest. It works really
well.

Anyhow, hope that gives you some ideas, for what it's worth.

Trying to program a barrel using a ball and negative thick would only work for open angles.  Once the contact point moved to the top half of the barrel you'd be screwed.  :(

Yeah, I've never tried to program a barrel. It works well for the tool with
larger bottom radius than the diameter, though. Funny- we use these tools a
lot, but never know what the "official" name of the tool is...I don't even
know if you can buy them. The shops I program them for grind them in-house.

In Reply to Bryan Carpio Felsher:

P.S.  I drive T-slotters all the time in MAFC.  I just lie and use a regular endmill and a user rep.  Works for me, but yeah...don't see why it can't be done by default.

 

Again....ALL cutters should be available in ALL MO's.  All macro's should be available in ALL MO's as well.

 

Anyhow, hope we get this new tool description.  I've done it a bunch, but it is kind of tricky.  In MAFC, I'll use a 2" ball with a user rep and a NEGATIVE offset on drive surfaces.  It works well.

 

I have programmed may times T-Slotter with MAFC to cut negative draft walls and it works fine for me. The trick is to change the cutter for the MO and I believe I had shown it somewhere here before.

As far as barrel, what we need is for CATIA to compute toolpath when the contact point switches from the bottom to the top of the cutter.

This requirement is also needed for T-sloters and lollypop type cutters.  CATIA should compute the toolpath no matter how many times the contact point switches from top to bottom or bottom to top.

So, if I can summerize and step back some from the details......

Any cutter with any MO has been discussed many times and would be a significant task for DS to accomplish. Perhaps not a realistic thing to expect DS to do.

Special shape cutters are used in production. I suspect that CNC cutter grinders make odd shapes affordable and accurate. A way to program these tools is needed.

In the real world there are multiple CAM systems under one roof. Managing NC cutters is a continuing problem that ISO 13399, STEP-NC, etc may or may not help.

I think, as I have said before, that a generic NC tool assembly definition (holder, adapter, cutter, meta data) is necessary, something all CAM systems can understand. I'm thinking that the geometry would be defined as a 2D profile using very basic point, line, arc, spline data. Something that just popped into my head is why not use APT do define the profile!!!! Taking an APT program and creating CAD geometry from it was done decades ago.  Piece of cake.

Once the assembly profile is defined there are cutting and non cutting portions. The cutting portion could be further refined as to which element(s) of the profile should be used for tool path computation. A single point on the profile could also be specified.  Other cutting elements would be ignored except for verification/collisions. This would allow any shape to be used because the "illegal" portions could be ignored.

Another approach could be similar to the CNC technology of running off the point on the part and the surface normal and compute the tool tip on the fly from that.  If you look at any point in the tool path there is a plane that contains the surface normal and tool axis. The direction of motion is normal to that plane. In that plane the tool tip can be defined from the point using the two vectors, regardless of the shape of the cutter, if the geometry is known.  So, you create a tool path that is normal to the surface, define the parameters describing the tool tip relative to that point, then the final tool path can be created.  I think this is exactly what is done internally with normal shape cutters.  By going right to the details (where is the tool tip?), the shape of the cutter is irrelevant.

I think this approach of adding a new tool type to all MO's solves a lot of problems. But, it creates new problems of getting all CAM vendors and cutting tool manufacturers to buy into it. It seems more do-able that the ISO or STEP type solutions that are not focused on NC programming needs only.

Something to think about.

I like your thinking, Jim.

Some of you may not realize, but this tool (say a 1" dia endmill with a 3" bottom radius) is 100% possible to define and drive in APT or NCL.  You can't put the corner radii in APT or NCL, but when I program these tools, I don't care about that, and it's not even taken into consideration.  You're driving the bottom and the side of the tool.

Once again, something that was possible more than 40 years ago, is not possible in Catia...I don't think that's right. 

I think you're on the right track, Jim- and I think yours is the best idea yet.

I wish they'd just simplify the whole problem and add a new cutter type and call it APT cutter.  Any tool that can be defined with the standard good old 6 parameter CUTTER statement can be used in any MO.

I think some of you would be surprised to see what types of tools were possible in APT with their standard 6 parameter CUTTER statement.  It really is very powerful.  When you add CUTTER/OPTION,(1,2),(ra,hi,OFF) the sky's the limit.  This is the "ring" cutter that Dave Frank described.  But you didn't even need that to make the special tool we're requesting.

A standard APT cutter statement is:

CUTTER/d,r,e,f,a,b,h

d=tool diameter

r=radius of corner

e=distance from tool caxis to center of r

f=distance from tool endpoint to center of r, parallel with tool axis.

a=angle from a radial line thru tool endpoint to lower line segment in positive degrees

b=angle between upper segment and tool aciss in degrees, positive or negative.

h=cutter height.

If e,a,b = 0, d<2r, f=r then you get the special tool we're asking for.

if e<0, f<r, a>0, b<0 then you get a basic "barrel cutter"

So...APT had BOTH these special tools 40 years ago, and could drive ANY series of drive and check surfaces....can Catia do that?  Too bad APT is dead!!!   lol...

In Reply to Jim Barkelew:

So, if I can summerize and step back some from the details......

Any cutter with any MO has been discussed many times and would be a significant task for DS to accomplish. Perhaps not a realistic thing to expect DS to do.

Rather then saying if I want to mill with a tap, let me do it, lets say I have a REQUIREMENT to drive a FAILSAFE PIN, with a Tap, and a Thread mill, and a Centerdrill. Hmm perhape we will get a seperate MO, just for that.

Special shape cutters are used in production. I suspect that CNC cutter grinders make odd shapes affordable and accurate. A way to program these tools is needed.

This is the meat of the issue. We must use these cutter, and CATIA has not direct methodology.

In the real world there are multiple CAM systems under one roof. Managing NC cutters is a continuing problem that ISO 13399, STEP-NC, etc may or may not help.

I think, as I have said before, that a generic NC tool assembly definition (holder, adapter, cutter, meta data) is necessary, something all CAM systems can understand. I'm thinking that the geometry would be defined as a 2D profile using very basic point, line, arc, spline data. Something that just popped into my head is why not use APT do define the profile!!!! Taking an APT program and creating CAD geometry from it was done decades ago.  Piece of cake.

My guess is in the code, there is a case logic statment

when/ cutter_style.equals.Ballnose, then

when/ cutter_style.equals.Bullnose, then

when/ cutter_style.equals.bell-conical, then

when/ cutter_style.equals.cone-conical, then

when/ cutter_style.equals.centerdrill,

thenwhen/ cutter_style.equals.tap, then

I could be wrong, but I doubt that 2d profiles are feasable. I could be wrong, but I think all cutter defs, need to be "Offical" with code writtent to do machining, replay, colision detection, and Video.

Once the assembly profile is defined there are cutting and non cutting portions. The cutting portion could be further refined as to which element(s) of the profile should be used for tool path computation. A single point on the profile could also be specified.  Other cutting elements would be ignored except for verification/collisions. This would allow any shape to be used because the "illegal" portions could be ignored.

Another approach could be similar to the CNC technology of running off the point on the part and the surface normal and compute the tool tip on the fly from that.  If you look at any point in the tool path there is a plane that contains the surface normal and tool axis. The direction of motion is normal to that plane. In that plane the tool tip can be defined from the point using the two vectors, regardless of the shape of the cutter, if the geometry is known.  So, you create a tool path that is normal to the surface, define the parameters describing the tool tip relative to that point, then the final tool path can be created.  I think this is exactly what is done internally with normal shape cutters.  By going right to the details (where is the tool tip?), the shape of the cutter is irrelevant.

I think this approach of adding a new tool type to all MO's solves a lot of problems. But, it creates new problems of getting all CAM vendors and cutting tool manufacturers to buy into it. It seems more do-able that the ISO or STEP type solutions that are not focused on NC programming needs only.

Something to think about.

Yes it is interesting. I fill be fun to see what the developers think of this, at next years annual conferences discussions. wow... just 8 months away. Soon the deadline for presentations will be due.

Nice comentary Jim,

 

Dave

Hmmm,

 

I tried to review the ISO 133399 standard, and it seems they want you to pay good money to even look at the damn thing.If somebody has a link to a good detailed explanation of what this standard really has to offer, please share.

Sorry, but I get a chuckle every time someone mentions STEP-NC. I've been told for the last 30 years that N/C Programming is going to be automated out of existence. 

My vote would be for the 10 Parameter cutter over the APT 7 Parameter cutter. It gives you much more flexibility of the tool form that can be described.

  Randy Hitzeman

Something else we had in APT that I miss is being able to change the cutter definition without doing a tool change.  It seems like we should have more fexibility to define temporary cutter shapes that are used just to create motion.  But we shouldn't have to define a new cutter assembly and tool change since it's only for programming and no info needs to be sent to the machine about it.

Thanks everyone for their effort.  This is a very important topic

I agree Roger. That was a very good feature. I've actually done it in
Catia...sort of. You create the new tool, but you "Deactivate" the tool
change. It works pretty well. Very rarely have I found that doing this was
worthwhile, but I've done it before and it works. Sometimes I used to do it
to change the offset on drive surfaces before I could mass-edit MO's using
my VB script. For instance I decided I wanted to leave .002 on all drive
surfaces for some toolpaths. I'd create a "dummy" tool .004 larger in
diameter, replace the tool used on those paths, then deactivate the tool
change.

It's kind of mickey-mouse, but down and dirty it got the job done fast, when
that's all you care about.

I agree with this also.

Call it an "In-Process Cutter", or a "Psuedo-Cutter", a "Synthetic Cutter" or whatever.

Maybe this would be the easy way to get around the limitation of not being able to drive a reamer around a failsafe pin. 

You would have to have the option of retaining the initial cutter's "User Representation".

There would also need to be some sort of "Flag" on the operation that the false cutter is actived on to identify them.

 

Randy Hitzeman

I was thinking about how Catia could already build a cutter from an APT definition, sort of.  It does this when you "Import APT"- builds a cutter from the CUTTER statements in the APT fileyou import.  At least a step in the right direction to getting our new "APT Cutter" definition....dream on...

This is a top three in my opinion.

---

Dave Frank

COE Product Chairman, Digital Numerical Control

Do you folks think this is a top ten?

I do  ....

---

Dave Frank  *    Bell Helicopter *  Grand Prairie Texas

Advanced Computer Aided Manufacturing Systems Engineer

COE Product Co-Chairman, Digital Numerical Control

 

No, but I think that an APT style 7 parameter cutter IS, with CUTTER/OPTION,x (to create a "ring" cutter) IS a top 10.  With this ability, your cutter would be possible, along with a LOT more cutter styles.

I'm sure they could get the code pretty easy for this...APT360 is now public domain....I have the fotran and C source code (even compiled it on my Linux system and it works!), and they can have it if they want...what is it- 40 or 50 years old?  Yeah, I think Catia should be able to do it...drive and use any combination of 7 parameter cutter with any Drive/Check/Part surfaces...

Bryan,
I believe you might want to say 10 parameters becsuse Catia has kind of 7 parameters cutter statement and it can be observed when importing aptsource file. But that functionality cannot be used efficiently to build a new cutter definition by the user. 

I would definitely like to see 10 parameters cutter def. and I have already sent the catpart for it to DS R&D with all the formulas inside it. I think have posted the info somewhere here before. 
Vericut has it, Ug has it, why not Catia

Regards,
Samarinder Singh

-------- Original message --------
From: Bryan Carpio Felsher <[login to unmask email]>
Date:
To: [login to unmask email]
Subject: [manufacturing] - RE: Need2 define a Cutter, with a large spherical radius, ALSO be able to drive Barrels mills with MAFC

No, but I think that an APT style 7 parameter cutter IS, with CUTTER/OPTION,x (to create a "ring" cutter) IS a top 10.  With this ability, your cutter would be possible, along with a LOT more cutter styles.

I'm sure they could get the code pretty easy for this...APT360 is now public domain....I have the fotran and C source code (even compiled it on my Linux system and it works!), and they can have it if they want...what is it- 40 or 50 years old?  Yeah, I think Catia should be able to do it...drive and use any combination of 7 parameter cutter with any Drive/Check/Part surfaces...


Site Links: View post online   View mailing list online   Send new post via email   Unsubscribe from this mailing list   Manage your subscription  

Use of this email content is governed by the terms of service at:
http://www.coe.org/p/cm/ld/fid=2

37

In Reply to Randy William Hitzeman:

Dave,

The first priority on my tool wish list would be the large radius bottom tool, hopefully with corner radii included. I don't think I've programmed for a shop anywhere that does not use this style of cutter. We really need to impress upon the developers just how common and widespread the use of this tool is.

A lot of people may be unfamiliar with the barrel cutter, so I'll have to do a history lesson.

The barrel cutter came from Douglas Aircraft. Because of their resident genius, Paul Mills, Douglas was the first aircraft company that had mathematically defined loft surfaces in a computer format. They also had an extended APT add on program called DAC-ARLEM that could take advantage of these mesh defined surfaces.

The barrel cutter was developed to efficiently cut inside of a concave surface. By specifying different cutter contact height for the barrel cutter, the concave surface could be cut in just a couple of passes. What would take 50 or more passes to keller with a ball nose could be done in 3 or 4 passes with a barrel cutter.

 Paul Mills later developed NCL, so that's why NCL has barrel cutters. McDonnell Douglas's McAuto division at one point owned Unigraphics. That is why Unigraphics has a 10 parameter cutter definition.

Those that programmed outside of the Douglas sphere of influence may never have used a barrel cutter. Boeing had their B-Surf routines, but compared to what Douglas had, it was quite lame in comparison.

 

When Dassault licensed NCL's tool path strategies, I would have thought that the 10 parameter cutter statement would have come along with it. And then when a barrel cutter definition finally was added, I would of thought that the first and most logical operation to use it in would have been MAFC. MACF is where the barrel cutter should be deployed, it's useless anywhere else.

 

Randy Hitzeman

Hi Randy,

 

When I took my first NCL class....1986?.... Paul Mills's son was in the class. John Gates was the instructor, and a excelent one. Facinating history lesson between you and Jim.

The spherical cutter and Barrel Cutter are top Tens from 2013.  No one has provided a use case for a 10 Parameter cutter. I did a webinar on it and asked.

This is a cool thread.... it reminds me of the good old days when the forum was on fire, and all the good old guys were banging away.

 

Dave

 

---

Dave Frank  *    Aerospace Dynamics International, Valencia, Ca

5-Axis CNC Programmer

COE Product Co-Chairman, Digital Numerical Control

 

I agree that the large bottom radius cutter is a top priority.

Every shop that I've ever worked in has used them.

My preference generally is to use a bull nose cutter with a lead angle, but this usually requires a multi-axis machine.

If you don't have one, or the surface is too complex, your only viable option to efficiently keller the surface with a large bottom radius cutter.   

 

The barrel cutter end mills have kind of gone by the wayside I'm afraid.

Outside of the McDonnell Douglas sphere of influence, no one else seemed to use them.

The reason being that only DAC-Arlem and NCL supported them on the programming side.

High speed machining and more powerful graphical programming have also negated a lot of their appeal.

Randy Hitzeman

In Reply to Dave Frank:

Hi Friends,

We, and I mean you, and I and all of us, Need to define a Cutter, with a large spherical radius, and......also be able to drive Barrels mills with Multi-axis Flank

We have a requirement to machine a part with a 1.25 Dia cutter with a  5 inch spherical radiuson the bottom. But there is no method to define such a cutter as it truly is. People do use workarounds.  Lie and then use a user rep, ... but that requires containment sketches, and messes up automation for shop docs, and you say 10 inch dia Ball, when it is really a 1.25

What a cutter like this is good for is for machining parts with a small amount of curvature. Everyone I know has used these tool for years....This is very efficient, and reduces the amount of hand grinding on parts when done.

This could be both 3 and 5 axis. You can imagine that the same result of finish would be gained by either 3 or 5-axis… and the reason for wanting 5-axis would be to tilt a little to no cutter with the area of the tool near the center line, that is usually going very slow constant surface speed, and also… if you need to tile of he floor is at a steep angle.

This is a very important function, as this is a STANDARD tool for the aerospace industry.

We define this kind of tool in NCL by saying I have a 6 inch diameter 3 radius ball with .0658 height. The height makes the tool what we call a disc. Note in NCL the side .125 rad not defined in this method

This tool is also definable in UG-NX.

++++++++++++

Another topic that is related is to be also be able to drive Barrels mills with Multi-axis Flank. I like the new tool definition. I know sometimes DS will give us a new function... like the new Barrel with limited usability, and request Feedback.

My feedback is the next MO I would like to see barrels used on is MAFC.

I have Vetted this enhancements with a few friends, and all agree this is important functionality, so I hope DS can plan to put some people on it.

In the mean time, I hope you COE members, can help define the requirements in more detail.

Best Regards

Dave

 

 

Hi Fellow NC Programmers

You can now  drive Barrels mills with MAFC in V5

Thats V5, 2016, which is available

2015 SP4 is also available now, and has a improvment in concentric roughing and pocketing

Dave

---

Dave Frank  *    Aerospace Dynamics International, Valencia, Ca

5-Axis CNC Programmer

COE Product Co-Chairman, Digital Numerical Control

 

Hi,

What happened to this Barrel Cutter in MAFC. I still don't see it in R28.

I'm using V5 R2018 SP6 (PLM express) and can't use a barrel cutter either. Any reason why? 

Found this!!

Thanks for info Tony. It turned out to be a different variable. 

Thanks Tony! Actually our DS friends gave me another variable to activate the Barrel Cutter in MAFC inside R28.

Can anybody tell me what the name of the variable is for activating in MAFC. I'm working in R29.

Eduard De Smaels - Technical Adviser CAM Engineering

ASCO Industries (Belgium)

MFG_5XFLANK_BARREL_TOOL=1

This works !

Thank you

Eduard De Smaels - Technical Adviser CAM Engineering

ASCO Industries (Belgium)

We are using version 5-6 release 2019

Build Day: 06-20-2019.20.00

Service Pack 3, Build number 29

What version do I need to update to to use the lense cutter. I do not see it as definable in this Version.

 

Thanks,

Kevin C.

It's available in V5-6R2020 SP1 in Sweeping, contour driven, spiral milling (with 3 to 5 converter), in multi axis spiral milling with the variable 

MFG_ENABLE_LENS_TOOL

In V5-6R2020 SP4, it will be also deployed in multi axis tube and multi axis helix.

Hi Samarinder,

I tried all the variables listed in this thread to use a barrel cutter in MAFC MO in R20. Just wanted to know which variable did you use. Please let me know.

Thank you

Mohan