Machine won't cut out my part!

[SpeedsCustom]

Ok hello everyone, I need your help. I designed this small parts for my brothers Rc Car. I designed this in Pro Engineer, saves as STL and transfered too Meshcam for the G-Code. I originally had set the Roughing pass with a 5/16 end mill, the finish and the pencil clean up with 3/8.

Before I go on, I can do pictures, but it's parts I design I want too cut!

Ok...So I set up my stock using the software saying that the total leng was 97mm (x) 12 (y) and 13 (z) the actual part is 90mm (x) 8mm(y) and 4mm(z). I set the stock up bigger because when testing different lengths of stock, when I generated my path there would times where there was much more lines then other, so I thought oh...it must not be thinking the Stock is large enough so it won't bother too cut that part.

After I set it up, or so I thought?....I ran the mill.


I offset the Z 9mm because the part I milling, I was hoping would fall out the bottom since I said the stock is 13mm and the parts is 4mm, well in any case, it looked like it was going smooth, and then after a while the program ended and all I had was the top surfaced down to I guess 4mm and then one of the sides "Slightly" contoured, but only one side and not enough too make it look good.

Here is what the parts is suppose too look like.



Am I better off milling the stock down too 4mm thick and trying too run it so it just cuts out the piece without it surfacing and everything.


Also, it never asked me too change tools, did the program not finish?


-Speed

[SpeedsCustom]

I'm going too enlarge the stock, i just generated new path and seems like it will cut more. We'll see.

-Speed

[LeeWay]

Is it a demo or evaluation version? I have Meshcam, but haven't used it that much yet. If it is a demo, it may be limited to a certain amount of gcode lines. If you have purchased the software, go to Help About and make sure it recognizes you.
After a reinstall once, I had to re register the code number that was sent to me originally.

This is one nice thing about Meshcam though. You can have a block of material and mill a part out that is hidden deep inside. Much like a famous sculpture once said about his work. I take a block of marble and remove everything that isn't a sculpture.

[ger21]

Are you talking about roughing, finishing, or both? It won't rough correctly if the depth per pass is too high. And make sure the stock is bigger by at least the tool diameter if you want it cut all the way around. I need to see a screenshot with the toolpaths if possible. Are you using a 3/8 ball tool? It may be too big for that part.

MeshCAM is really not the right tool for that part. Something like SheetCAM can do that with a 2D drawing far faster than MeshCAM will. And it'll probably need less than 5% of the code to do it.

[SpeedsCustom]

It's a demo, but i was told it does not matter. I have generated codes in meshcam having over 10,000 lines.

Ger21-Kinda both, I had set the Path too rough and finish it. I was "going" too use a 1/8 endmill. I meant too say 1/8 not 3/8! Oops.


I thought Meshcam was capable of cutting actual parts out I was planning on using Meshcam for my my designs.

-Speed

[ger21]

If you post your part, I'll show you how to do it. MeshCAM can cut parts just fine.

But for that type of parts (2.5D), there are better alternatives available. Meshcam excels at cutting freeform shapes. Parts that are basically cut from flat stock can be done much more efficiently with a 2.5D package.

[ger21]

Are you using a demo of mach3 by chance? There's no limitations with MeshCAM's demo, but there is with mach3's.

[SpeedsCustom]

No i'm using EMC2.

I think I just left too little stock.


-Speed

[under-dog]

Speed,

I mentioned in another thread as well(the one with the Burton plate). But figured worth mentioning here too.

For the types of parts you are looking at you are better off using a 2.5D toolpath strategey. You will get much more efficient files and much cleaner parts. In fact you will not even have to solid model something like you have shown. A simple DXF will do. I realise that The part shown is just an extrusion but...

The toolpath file will be far easier to make as well. 2.5D
contouring and pocketing do not care about stock sizes and such they just cut the toolpaths where you tell them as you tell them regardless.....

Someone else said it her already thet meshcam is a 3-D raster strategy program and is better suited for cutting things of a more sculptural freeform nature.


If you are still in the trial version then it is not too late to go to a program that is more suited to your type of parts.


Dont get me wronge Im not dissing Meshcam. I owmn it and use it for my 3D sculptural projects. But I also use desk CNC for all of my parts that are similar to what you have shown. All the upgrade parts in the thread I did on my upgrades are donr this way.


If you would like i can elaborate on the differences in the tool path startegies I mentioned. Just in case you are aware of the differences.

[SpeedsCustom]

Would I be better off saving it as DXF and importing it into Meshcam?

I'll get back too this thread.


-Speed

[under-dog]

Originally Posted by SpeedsCustom Would I be better off saving it as DXF and importing it into Meshcam? I'll get back too this thread. -Speed

No

See thats the thing. MeshCAM works strictly with 3D data (STL files and 3D DXF). So it would still have to be a 3D DXF. So it analizes the enture surface data and generates tool paths for that entire surface. You may only be making one hole in a flat piece of stock, for example, but it will have the tool cutting the entire part surface just to get that one hole and doing so in a raster fashion. Raster will give you a poorer quality cut in this sort of instance.



A 2.5D program that contours and pockets uses an entirely different logic to how it generates tool paths. You use a 2D DXF and select the different geometric elements or "profiles" (In the case of your part: two holes and the rectangular border with rounded ends) and specify the cutting parameters for that specific area. The holes would be told to cut to the inside and up to your line, to your desired depth (thickness of your part + a little) and the border to cut to the outside in the same fashion but to the outside. The tool paths created would generate just what is needed to make the two holes and the border.

The tool moves by following your geometry not by going back and forth and making plunges as needed (raster).

It dos not care if you are cutting this hole into a plate of aluminum or your wifes favorite china, it just knows to "follow this line to a certain depth"



There is a similar thread going on right now that is discussing pocketing and contouring:

http://www.cnczone.com/forums/showthread.php?t=49837


If I were you I would really look at a 2.5D software package as well if those are the types of parts you will be making. I try to use 2.5 D over 3D rastering whenever I can much cleaner, faster and efficient. Desk CNC will do both it is just not as advanced or as many options for the 3D contouring as MeshCAM. They offer free trials on those as well. Get a trial and just try cutting a simple hole to see what I am saying.



Just thought of this: contouring and pocketing basically does just the pencil cleanup portion of what you have been cutting now without all the back and forth over your entire surface while not actually cutting the top of the part. In the case of your Burton plate it would have ignored all your top surface(doest even know they are there) and just cut your lower portions in. You can still have it remove all the material in between your borders(this is called pocketing).

In the part above it would have cut two holes in and then traced out the outer edge and the part is done.

In the case of you stock being too thick as you mentioned. You either start with a more appropriate stock size or face mill it to the proper thickness before cutting your profiles.

[SpeedsCustom]

Wow, great thank you so much. I knew there had too be an easier way of cutting the parts. I just felt that is did "Unnecessary" things, going back and forth for no reason. What you mentioned in your last line is perfect. I would first make the stock 4mm and then run the program too make the holes and just cut out the part. Thats what I need.


Other then DeskCNC, could you recommend any other programs I could maybe buy without killing my wallet ?


-Jason