Do CNC programmers really need to change your SolidWorks models?
I was at a customer site recently where they were trying to streamline their process. The CNC programmers had several complaints about the models the SW users supplied. Hearing that complaint is nothing new, but what is difficult about it is determining if the problem is really a CAM training problem, a CAD training problem, or if some other software would handle the situation better (or worse).
Looking at the models, I noticed a couple of things. first, the fillets and chamfers were placed willy-nilly in the tree (they weren’t all at the bottom), and some of them were sketched rather than placed as actual features. Sometimes you really do have to do things this way, but I think these models would have been better with features. I also saw that some of the chamfers were on inside corners (red faces) so the only way to create them was with a broach or a file. This was certainly unnecessary and kind of thoughtless on the part of the designer.
So what do CNC programmers do when they use a standalone package and get a translated part? You can’t complain about feature order there. Do programmers really need an edge to be unbroken in order to machine that face? On the image shown, that would be the vertical face below the orange angled chamfer. That’s an honest question, no sarcasm. Does the machinist need to remove the orange chamfer before he can program the vertical face below it? I suspect the answer is “no”, and a CNC programmer that demands unbroken edges probably needs training.
And then what about non-orthogonal edges that have fillets (yellow in image), and you only have a 3 axis machine? Do you really need to sculpt face of the fillet with a ball-end mill? The fillet is truly an arbitrary edge break on machined parts, and it seems like such a waste to throw so much time and effort into something that matters so little.
And what of the orange face? If you only have a 3 axis machine, a regular chamfer tool will not cut that face without repositioning the part. What do you do there?
And then on the drawing, how do you communicate ‘I don’t care what you do’ when it really doesn’t matter?
What’s the difference between CAM software that runs inside SolidWorks and standalone CAM software? I assume the ability to see sketches and features counts for something.
Further problems at this engineer-to-order manufacturer were that sometimes the parts that came out of the engineer-to-order process this week were the same exact parts that came out of the process last week, but with a different customer and different part number. How do the machinists avoid reprogramming and re-setting up the same exact parts? This seems like a vulnerability of the engineer-to-order process. Any ideas?
“And then on the drawing, how do you communicate ‘I don’t care what you do’ when it really doesn’t matter?”
RADIUS TO SUIT
CHAMFER TO SUIT
DRAFT TO SUIT
Devon
I’ve never put a feature on a part where I didn’t care what the machinist did with it. I may have rather loose requirements expressed with a large allowable tolerance or MAX/MIN callouts, but not a complete ‘I don’t care’.
I’ve been fortunate in the past to have a good dialogue with the programmers and machinists, where we’d work together to both learn what the other needed or wanted to make life easier – and produce better parts. Unfortunately manufacturing isn’t in house at my current employer, so I don’t have that feedback mechanism anymore.
I usually call the shop when I send the parts or drawings over and we go through any problem areas or tolerances. By working with them I find I get better service, better parts, better prices, and most importantly a happy machinist!
Solidworks will let you desing parts that are almost impossible to machine, but yet easy for injection molding or a different manufacturing process.
Understanding the way that parts are machined before how parts can be designed is a huge advantage. Don’t think about 3, 4 or 5 axis machines in general, but think about how the machine actually works removing material to create the part you designed.
If you actually needed the chamfer to be sharp in the corner, would it be possible to make the part as a 2 piece assembly? You will need 4 set-ups to cut that chamfer in the corner, not having to broach or file it.
This part I would send the machine shop an IGES or STEP file, one with the chamfer and one without. This is less confusing to any CAD or CAM software when having to program CNC machines. They need to program the part as set-ups, not as a complete part in one set-up.
As a Manufacturing Engineer who works with SW at a contract medical device manufacturer, I can tell you that there are times when I need to tweak the model in order to make it more machinable. Aside from basic import errors, many design engineers have apparently never stuck there head in a shop.
We often have to get approval for multi-pc weldments for things that can’t be made as a single piece. Sharp corners are frequent problems; and just plain poorly dimensioned prints (I often have to pull critical dimensions from a model). And don’t get me started on GD&T and the way people interpret that!
It amazes me sometimes what gets approved for production when someone like me, with NO machining background, can tell you that we can’t make that. If we didn’t make the prototypes, surely someone did, and no one apparently made a note of the issues?!?
The eternal conflict between design and manufacturing!
One way to avoid reprogramming and re-setting up the exact same parts is to have an internal part number for the program and set up that can be called out on the “new” customer engineered-to-order part. This would require the program that creates the engineered-to-order parts to keep track of previous part’s parameters and check to see if it already has been created, and then print out a list of manufacturing internal part numbers for the program and set up.
Doesn’t seem to difficult.
I touched on some of this recently in a manufacturability article. I look at the example and note the following:
3-axis mill machinist will have to move the part, or set some tooling to knock the chamfer down. The inside chamfer corner will have to be dressed by the debur-girl (or guy..whatever) with a file.
Ball mill will profile that Fillet.
I think there needs to be some general understanding between both Design and Machine folks. One company I really liked had a team that was integral to their process and took the designs and tailored them to that company’s processes. Very clean operation.
If the feature is needed, then apply it. Period. If it is desired, but not required, then state that much on the drawings.
Some features just can’t be run on 3 Axis. However some features can be tuned to be accomplished on a limited machine, if you, the designer, know about the limitations beforehand.
The machinist/CAM folks needing unbroken edges…..I hesitate to make a comment that will seem offensive to some. The point is do what you have to, imply flexibility where you can, and let the people downstream earn their pay.
CAM Express (from Siemens) has Synchronous Technology. With Synchronous Technology, the CNC Programmer can modify or even remove the blends.
With Synchronous Technology, it doesn’t matter what the order of the features are.
Plus, CAM Express can maintain full associativity to the original model so that if the design changes (and we know it will), those changes are automatically incorporated into manufacturing.
An example: A pocket has a corner radius of .250″, and the CNC Programmer will use a .500″ endmill to machine it. He knows the radius has a +/- .030″ tolerance, so he modifies the radius to .265″. That allows the tool path to “drive” the corner (reducing chatter) yet still maintain the design intent.
You can see Synchronous Technology in action at this link: http://www.youtube.com/watch?v=PO_vRvioT4M
The only real problem I see in producing this part would be where the 2 chamfers meet in the inside corner. It could be ball milled, but the inside corner would have a radius to it instead of a perfect chamfer. This is where a conversation between the porgrammer and the designer would need to take place. And while that conversation is happening, you would want to ask if the other fillets and chamfers are really needed and explain why you are asking the question. A ball end mill could create both the angle radius and angled chamfer. They just take a little more time to make.
As far as stand alone vs. integrated, I don’t see it making any difference. The important thing is to get a solution that works. I don’t care where in the tree a fillet is. The only times I have ever looked at a sketch is to see what the radius for a sketched feature is for a complex feature when the measure command won’t give you an accurate reading for the feature.
Engineers that I used to work with tried to design their parts in the same way they would be machined. They would start with the overall size of material needed and then remove features to create the final part. This made them think more about how the CNC machine would make the part.
As a CNC programmer (primarily), I run in to this all the time. Just last week I got parts from a client who has been in the designer and engineering field for 20 years and yet still I had to work with him for a few hours to get parts that were what he wanted but didn’t require 5axis or many refixturings. When I get drawings from solidworks users that have never made a part before, they are almost always a disaster. They are usually either over dimensioned or incomplete. Unless there is a complex surface to machine I prefer to work off of 2D DXF files rather than the SW model as in CAM it is easier and faster to program. As for broken edges, I can work with them on the model but I prefer them unbroken with a call out as I am usually going to program my profiling end mill to run tangent to the outer edge of the part. The last complaint is the number of surfaces I come across that are very poorly built. Often importing them into cam there are anomalies and holes that I wind up having to fix before I can machine. I attribute this to laziness on the part of the modeler.
@peter
I am curious – what CAM system are you using?
@peter
Geez, 2d DXF sounds so barbaric. I’ve often heard machinists say this, but then I’ve heard machinists contradict it as well. I would hesitate providing that kind of data mainly because it is disassociated from the original file and it erases much of the advantage of 3D to begin with.
I think engineers need to have an eye open to the mfg process, but they should not be determining how a part is machined. I’m not sure why there is such antipathy between engineers and machinists, especially when they work for the same company.
I’ve seen the same argument up close with plastic parts. As a part designer, I do not specify how the mold works, but I need to design parts that are moldable. It requires dialog and understanding. I started this conversation mainly to try to understand the difference between real machining requirements and personal preference.
“And then on the drawing, how do you communicate ‘I don’t care what you do’ when it really doesn’t matter?”
For each callout, after the size, put “OPTIONAL”.
Who says the part has to be oriented with the mill with the z-axis up in the pictrure? Rotate the part 90° to avoid kellering the angled surface.
Smart component design is all about feasible manufacture, in as few steps as possible to achieve desired functionality.
I started off in the trades as a tool and die maker, working summers with my father at the age of 15 and then moving into CNC due to computer aptitude and a great deal of interest in the trades. I soon picked up AutoCad and taught myself how to use it; later on moved to Solidworks and 3d modeling. My manufacturing background and my ability to design complimented each other quite well as it seemed that many designers had such poor understanding of feasibility in design. I then decided to go to engineering school and have been working on that end ever since, primarily as a ‘Manufacturing’ Engineer, though my degree is in Mechanical.
I’d offer this advice; if a feature could be labeled “optional”, then simply leave it out. If it isn’t needed, then it only increases the cost of manufacturing the component… no need in even denoting it on the print. My first questions when looking at any component to be machined is, “Where is the assembly?” and “What is it’s functionality?”. So often we receive components that are overly complicated when a much simpler design would suffice, at a greater end profit to the manufacturer!
Looking at the model in question, I’d probably machine it (3-axis machining center) just as it’s positioned with Z-axis perpendicular to the base. That covers the sloped surface, the yellow fillet and the red chamfers. I’d chase the red chamfer from the right-side of the model to the left (climbing) and cutting-left of the edge with the actual tool’s diameter, not a smaller “effective diameter”. That allows the floor chamfer and vertical edge chamfer to be cut in one toolpath. The problem? There will of course be a radius in the corner, where the two faces meet. Is it ok? Well, we’d have to make a call to find out but while we’re at it, I might ask if the bottom-edge chamfer is necessary at all, as that would eliminate a chamfering tool altogether.
I think the best thing any designer could do, is spend some time in the machine shop learning how to produce the components they’re designing. That would eliminate many of the issues a machinist might run into.
Let me clarify that the vertical chamfered edge will also be cut by the end mill that creates the flat section to the right in this model view. The chamfer tool simply chases the profile out of the part surface to produce the tightest corner possible. The smaller the cutter diameter (whatever is feasible at this depth) the better.
@Jim Wright
Mastercam mostly. I also do some contract work for a company that uses Gibbs.
@matt
Mat. The associativity can be hard to manage. There is something to be said to not having to reprogram a complex part from scratch but often I’ve had revisions that are different enough that enough of the existing tool paths fail as to warrant reprogramming anyway. I think part of the animosity between designers or engineers and shop folk stems from the misconception that the designers et al are some how above the programmers and machinists, and some times act like it. I have seen a lot of venom spewed (right or wrong) when poorly dimensioned shop drawings or impossible to make parts have hit the floor. Having managed the manufacturing division I have seen both sides and done both part modeling and the drawings for manufacturing. I will say however, in my last company I held a number of hour long seminar for the engineers on how to create a proper shop drawing and how to think in terms of how the machines cut so that they could design parts that could be made more easily. Within a week I was getting all the same complaints from the shop floor as if not one of the attendees had listened to a word I had said.
Associativity is wonderful when it works but more often than not, the changes fail to come across in the revised CAM update, just as Peter mentioned. I think you’re best bet for the highest degree of associativity is in employing packages which incorporate CAD & CAM like ProE/ProManufacturer, Catia, etc.. It seem that it’s better — associativity-wise — to extract the least amount of geometry possible but then, geometry extraction is often necessary for control which is paramount in creating efficient programs, so there really is no clear-cut answer there.
I’m a huge proponent of using 3d models in CAM, probably because I spent so many years programming complex multi-level parts from prints and later, .dxf files. Nothing quite like ctrl-clicking a floor to fill in a Z-parameter, or in this model, selecting an edge to drive a ramped tool path; if indeed you wanted to cut the orange chamfer that way.
That last part should answer: “And what of the orange face? If you only have a 3 axis machine, a regular chamfer tool will not cut that face without repositioning the part. What do you do there?”
A couple other things to keep in mind are; component material and scale. A 1mm chamfer is no big deal but a 15mm chamfer creates another issue all together. Step-down profiling with a smaller chamfer-mill is always an option but then there is the time involved in machining the feature, not to mention the tool wear associated with a process where the effective diameter change creates a compromised cutting speed/feed. Tougher less machinable materials only exacerbate the problem. Using a ball-mill — the only feasible alternative at some point, of course adds time to the process…
Short answer, yet again; if it isn’t needed, don’t model it in.