Effect of modelling method in CAD on CAM 3

[LCform]

Hi All

I am a noob in CAM, and have decided to learn producing G-codes , I am searching for one first conceptual question and I don't find it, that is, when I model my part first in CAD, should it be exactly modelled in the same way it's going to be machined ? or it's just about the position of the borders ? is there any specific difference like if you have a radius in sketch or you fillet it in 3D for example ?

The CNC I am refering to is 3 axis milling

 

[3DDave]

Probably. It depends. It is typical that one would want to machine the part so that tool wear will not result in out-of-tolerance parts. It is also depends on the cutting tech. For example, laser and waterjet cutters have a known kerf, and cutting on the nominal part profile will remove more material than expected.

The offset to this is that decent G-CODE controllers allow for tool offsets to make up for wesr and kerf and can even account, if told, for large differences in cutter radius.

 

[MikeHalloran]

I have checked G-code sequences by manually generating the cutter path in AutoCAD, from the G-code file, in 3D. AutoCAD does not natively understand G-codes, but it understands lines and arcs.
It's the sort of grinding stupid labor at which computers excel, i.e., it's boring, repetitive and not fun for more than half an hour.

If you are designing a part in CAD, just design the part you want.

Yes, you want to avoid things like sharp internal corners, but in general the CAD operator should not worry about what the machinist or the CAM operator is going to do.
Just get the geometry of the generated part right.

I.e., the CAD output file, typically a DXF file, describes the generated part.
The corresponding G-code file typically describes the cutter centerline path to produce that part, which of course assumes that the exact cutter to be used has been selected already, and the G-code file will require adjustment if the cutter size is to be changed.

That assumes you are using a fairly elemental machine control; some of the newer ones allow you to do CAD right at the panel, but unless the part is simple, that's probably not a good use of your time, or the machine's time.

Many CNC machines come with software simulators that you can install on a PC. They are great learning tools for what you seem to want to do.




Mike Halloran
Pembroke Pines, FL, USA

 

[tygerdawg]

should it be exactly modelled in the same way it's going to be machined ?

Generally YES as you should model your net shape requirements. Modern CAM systems provide automatic offset values to accommodate tool wear, stock allowances, etc. The skill of the programmer / machine operator helps when they set up the NC machine, too.

Many sources for online learning of G-Code, dig around and you'll find them.
For a CAM system, the Uni I'm with standardized on HSMWorks because it is cleanly integrated with SolidWorks. It is now an Autodesk product so is also ported to Inventor. I/we like it because ease of use, integration with SW, and is designed so that a simple mouseover of the commands pops up a very good explanatory note. And if my info is correct, they offer a free HSMWorksExpress version covering 2-1/2D CNC. Somewhere on the HSMWorks site / Autodesk site you can find a web-based version of something called CNCBOOK. For newbie CNC programmers like me, I found it very useful.

Then there is always 100's of knowledgeable (and opinionated) people with lots of experience about this stuff on sites PracticalMachinist and CNCZone.

TygerDawg
Blue Technik LLC
Virtuoso Robotics Engineering

http://www.bluetechnik.com

 

[berkshire]

Most modern CNC tools have pre-process controllers that can take the raw output from DXF and other files, generate an editable tool path, where you can check tool offsets and control sequences. With this the operator gets to decide which cut is done first, and with what tool.
B.E.

You are judged not by what you know, but by what you can do.

 

[LCform]

Thank you very much All for your kind attention

 

[dgallup]

I typically model the same as a part will be produced but it's not because of CNC programing. Many of our parts are designed and tooled once and produced for years or decades. They tend to be made on multi spindle screw machines so setting up each machining operation is very important. We make operation sequence sheets of each step in the process. By having the model features match the machining process I can just step through the features and have a model instance of each operation.

One thing that is important for CNC programing is to model at the middle of dimensions. So if you have a round or chamfer that says 0.3 max. on the drawing, you don't want to actually model it at 0.3, you have to model it at something less.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[LCform]

shall you very please upload one sample for me ? I want to evolute and find a standard way of producing machinning drawing , I will be so so grateful....................

 

[SwinnyGG]

Yes, you want to avoid things like sharp internal corners, but in general the CAD operator should not worry about what the machinist or the CAM operator is going to do.
Just get the geometry of the generated part right.

As a blanket statement I would disagree with this- although in some particular situations it may not matter, on complicated parts, as designers we can directly effect project lead times and budgets by making smart design choices that don't effect function but DO effect machine time required to produce a part.

The entire point of GD&T, after all, is to relay to the machinist or welder or casting plant or whomever which tolerances are important for part function, and which aren't.

Generally YES as you should model your net shape requirements.

Absolutely, for multiple reasons- especially now that CAD models are often used as a 'master' reference if there are questions on a drawing. In my particular niche, the CAD model is ALWAYS net shape, regardless of the process being used to create the part in question. This makes the process of referencing to the CAD model totally unambiguous, and also ensures that if that model needs to be viewed long after I have moved on to another project or another company, there will be no questions about whether I added or subtracted material in the model to account for machining tolerances or mold shrinkage or whatever.

 

[JayMaechtlen]

In the general sense, you should have some clue as to suitable processes that will or may be used to make your parts or assemblies.
It can really increase costs if parts are not designed for manufacture.
- but, that is a whole family of concerns and considerations.

Jay Maechtlen

http://www.laserpubs.com/techcomm