3D cam, how to use, setup

[kimfmx]

Hi,

I have mainly used 2.5D for some time, and is fairly confident in this realm, and thers not much optimisation to be done in this aspect.

So I have come to the interrest of 3D machining, and have come to a some vital questions.

I have tried MechCam, and must admit the result is not exactly what I expected. I was kind of hoping there would be some kind of intelligent software for machining 3D objects, instead of just running back and forth or doing waterline machining. (cant find a explanation of what pencil machining is).

The finish or going back and forth in X and Y does not give a nice result.. What Im thinking, is how does a MAjor company make a organic part using CAM software.. im sure a round object is not done by running back and forth in X and Y, but is actually done by running in a round pattern.

Another question is, if I have to go in X and Y for the finish, is there some good hints to size and type of tools to use for roughning and finish, and what about the passover, too small passover will makemy computer run for 100 years??..

Included is a part I want to make in STL Format, its very difficult for me to produce a result I was willing to send to the machine.

Any help or hints much appriciated.

[ger21]

I was kind of hoping there would be some kind of intelligent software for machining 3D objects, instead of just running back and forth

There is, but instead of $200, you'll need to spend $1500-$3000-or more. And you can't use .stl files. When a CAM program opens an .stl, all it sees are triangular faces. It can't recognize features in an .stl file.

You need a program that can accept your solid model in it's native format, or perhaps IGES or STEP, where it can detect features and follow those features.

Another question is, if I have to go in X and Y for the finish, is there some good hints to size and type of tools to use for roughning and finish, and what about the passover, too small passover will makemy computer run for 100 years??.

Depends on the material your cutting, I guess, but for a good finish, you typically want about 5-8% of the tool diameter for the stepover. The larger the tool, the larger the stepover can be. Ideally, for finishing, you want to use the largest tool that will still give you the detail you need.

What Im thinking, is how does a MAjor company make a organic part using CAM software.. im sure a round object is not done by running back and forth in X and Y, but is actually done by running in a round pattern.

A round object is not what I'd call an organic object. An "organic" shaped object is typically cut the way MeshCAM does it.
for a truly "round" object, yes, it would be far more efficient to use toolpaths that match the shape.

You might want to look at Visual Mill or OneCNC.

What CAD software are you using?

[kimfmx]

Im using Autodesk Inventor, and just looked, and it supports saving the file in the following formats:
DWF, IGS, SAT, STEP, STL, XGL, ZGL

yes you are right, I didnt meen organic, just a shape that would be recognised, like a round solid object.

You mention VisualMill and OneCNC, Are these softwares able to do a good toolpart from a STEP File or other contour contained files, or do you have other suggestions to good software.

I googled for what others use for stepover value, and have somewhat got the idea, so im using too large stepover values... however I feel that using the x and y running back and forth is by far the optimal way of doing things, and will contribute greatly to the wearout of the machine.. imagine making many parts this way ... Your inputs are greatly appriciated.

Best Regards
Kim Mortensen

[ger21]

The two I mentioned are some of the lower priced packages out there. There are many, many more that will do what you want, with prices starting at about $3000 and going up. I don't use any of these packages, but you might want to look at.
MasterCAM
FeatureCAM
EdgeCAM
SurfCAM

[kimfmx]

I have been looking at mastercam on the net, and it seems to be able to handle good toolpaths from 3D files, so I think Ill try to invest time on learning the mastercam.

And i may very well be that I move from Autodesk Inventor to Mastercam if its works like I need it to work.

Best Regards
Kim Mortensen

[TheBigJW]

Originally Posted by kimfmx I have been looking at mastercam on the net, and it seems to be able to handle good toolpaths from 3D files, so I think Ill try to invest time on learning the mastercam. And i may very well be that I move from Autodesk Inventor to Mastercam if its works like I need it to work. Best Regards Kim Mortensen

I would suggest you avoid Mastercam if you are going to eventually pay for the software. The cost to stay current will kill you. Do yuorself a favor and learn something else. Mastrcam even charges more if you just want to rotate a solid model. If you are in a small market outside the US yor dealer will not use any kind of fair exchange rate based on any kind of bank rate. For pricing but will just make up a price list as they go based on the needs for profit. If you still buy this over rated software try to get a license in the US. They really only support the product over the phone anyway.

John

[kimfmx]

ok,

My scope is purely hobby, and im not a company and dont plan to become one ever. I just feel slightly annoyed that the software available for the hobbyist is so inefficient as to toolpaths and not overusing the axises of the machine.. its a homebuild machine, and done with the least cost possible.. using used parts on ebay etc, so if the cheap software is going to wear out the used parts on notime by running endlessly back and foth for every 0.25mm of my block - and doing this for the better half of a weekend continuously.. then its not worth it... there mist be some software available for the hobby people that is just slightly more inteligent than the meshcam like software.... if not.. there must be someone out here to take up the oppertunity of filling this hole of CNC software... that would kick out alot of the other cheap CAM products from the market..

Its just there is so much difference in seeing a 2.5D (pocket etc) toolpath, which is fairly optimized (well its up to the user), to go to the next level of 3D, and see the software just wasting your time and machine milage on silli operations.

Best Regards
Kim Mortesnen

[ger21]

Meshcam has a feature called check surfaces that let's you restrict areas to be machined. By using these, you can cut only the sloping areas, and use a 2D CAM program to pocket, profile, and drill the remaining areas. Not the ideal way, but a workaround you might want to explore.

http://www.grzsoftware.com/news/2008...heck-surfaces/

[Brewmeister]

I machined your part (using only the STL) using only 2.5 axis tool paths.
I think this part is a good example of a job that does NOT need 3 axis simultaneous machining.



This is the verification showing the 3 paths in colors

Blue: Blank ( I used a block )
Green: 5mm tool with 0.5mm corner radius. 1mm stepdown
Yellow: 2.5mm Ball. 0.25mm stepdown (Optimized* profile)
Orange: 0.5mm Ball. 0.1mm stepdown (using IPW**)

The first path with the 5mm bullnose has cut levels at each of the flat ares, with 1mm stepdowns between those areas. This way the flats are done after this path.

The second path with the 2.5mm ball cuts a profile of the part at each level. Since th 1st path removed all the blank stock.
*Optimized means that the cut levels are adjusted based on the steepness of the part. In the areas between the 2 red lines I drew in, the stepdowns are reduced to about 0.05mm. above & below that areas the stepdowns are closer to the programmed 0.25mm.

The last cut with the 0.5mm ball is set to only cut where the previous path left remaining material (i.e. in the corners). I used a 0.5mm ball because it looks like the smallest radii on your part are 0.25mm

The catch: I used NX (Unigraphics) which has all the cool extras like optimization & IPW (In Process Workpiece. which keeps track of the remaining material.)

However, if you follow a similar strategy you should be able to machine the part effectively with 2.5 axis machining and achieve the finish you desire without any extra wear & tear on your machine.

P.S. Pencil Machining (NX calls it Flowcutting) refers to cleaning out corners.



Best of Luck

[mcphill]

Originally Posted by ger21 There is, but instead of $200, you'll need to spend $1500-$3000-or more. And you can't use .stl files. When a CAM program opens an .stl, all it sees are triangular faces. It can't recognize features in an

Not true. You can get BobCAD/CAM v23 for about $800 (list is more, talk them down) and it is fully capable of machining off of an STL file. I do it all the time.

[jvangelder]

Ive used a variety of cam/cad packages and also recommend bobcad v23

And mcphill is right about pushing them on the price, infact i got my v23 pro + a usb dongle for much less then i would have ever imagined.

-Jacob

[kimfmx]

Brewmeister,

Impressive result I must say, but looking at this realisticly, some of the tools you are using is 0,5mm, I didnt even know this existed, it must be on the borderline to becomming a needle (-:

but from the picture I can see the problem im trying to find a solutionto. the round crcles are not nice round, as they were not made by a tool going around the circumference of the material.

The result you have there, what is the calculated tooltime adding all the tools times together. I have always known it is possible to make a good result using the back and forth method, but getting the resolution that will give nice result will generate such a big NC program that I will have to purchase more ram.

but please tell me more about the program used to generate this toolpath.

/Kim Mortensen