[slideleft]

Hi All,
I'm trying to mill this part out of a chunk of metal. Drawing created in Pro-E. My milling approach after facing top of metal and drilling holes is to use rough contour toolpath (1/8" EM). This works fine on outer surfaces, except... it doesn't create tool paths over the flat regions. This is not a problem for the very top (it has already been faced), but it is for anything below the top surface.
One tactic I was trying to use was to create seperate toolpaths for these regions using an artificially small tool diameter value (.002"). But, when doing this it changes the .125" tool diameter value for the other portions of the job (messing up it's paths).
Also, this block has several other parts on it (not shown) of different depths. Is there a way to limit cut depths individually (currently, shallow parts cut to the same depth as deeper cuts)?
Thanks in advance, and I might not be able to respond till tomorrow if you have questions (4th of July obligations),
Happy Independence everyone,
Jeff

[warrenb]

The part looks pretty straight forward. The holes are a bonus too because you can use them as locating / clamping features. The first thing I see is you will need to machine a clamping jig because this part will need to be cut in 3 operations. First I would drill the holes though the stock. Then I would cut the split in what appears to be the hinge. That gives you two good locating fixtures to cut the rest of the part from both sides AND you can use those holes to clamp the part to your table. One thing to watch out for is this part may warp big time because the walls are thin and you will be removing so much material. It may be best to rough cut the 'arc' shape and then drill and ream the holes. Don't be surprised if you cut 3 or 4 of these before you get it right.

[Superman]

1st work out what tooling you want and what features you want these tools to machine.

BTW - there is no real correct way to program, each part is judged indivdually and another person may attack it in a different manner.

I suggest before you start, place on separate levels, the solid, the surfaces-created from that solid, and curves-created from that solid.
and not to modify these in any way. Don't create curves from surfaces if you can ( double ups, trim errors etc quickly appear )

If you need to create extra geometry, copy onto a new level and then modify/add geom and also name it accordingly. Yes, you will be creating more geometry
I find it is best to use the original surfaces and curves and then add additional geometry to join with these, placed on a different level to assist how the tool behaves before and after cutting the shape ie. create geometry that may extend across stock to the part eg u to └u┘. Quite often this is overcome using lead in/out or extending / shortening

IMO- to start you off

1. Face top to finish size, say T1=3" facemill
2. create a contour boundary using c-hook "shadow boundary"
3. offset this new boundary by 50% of the cutter you wish to rough the shape with, say T2=1.5" tip cutter
4. 2D Contour-rough the excess material outside this #3 boundary ( remove corners, heavy cut areas etc. )
5. Rough Surface Contour, pick your shape, in "depths", set auto detect flats, and adjust stock on depths
6. Drill- do the holes
7. 2D contour,T3=4" side & face, in the area between holes, use lead in/out to make the tool clear the part, you may be able to use this tool for the other hole

[slideleft]

but... this part has radiused sides. It had been very easy to generate tool paths (forget holes and key slot, I got that part figured out) of exterior profile by selecting entire part and using 3D contour. I can do this for roughing(standard EM) and finishing paths (ball endmill). It was specifically with the flat regions that I am having problems coming up with easy toolpaths.
Thanks for your replies.
Jeff

[warrenb]

but... this part has radiused sides. It had been very easy to generate tool paths (forget holes and key slot, I got that part figured out) of exterior profile by selecting entire part and using 3D contour. I can do this for roughing(standard EM) and finishing paths (ball endmill). It was specifically with the flat regions that I am having problems coming up with easy toolpaths.
Thanks for your replies.
Jeff

You're going to have to use 2d profile and pocketingfor this part. There's nothing I see that requires a 3d toolpath. The edge break radii can be handled with skillful use of a file or deburing tool after the part has been cut.

What software?

[Superman]

What software?

DUH warren, what forum is he in ???

[warrenb]

DUH warren, what forum is he in ???

DOH!! What version? At least I can claim ignorance on that. Then in that case everything on this part can be 2D surface projections. There's nothing requiring 3D toolpaths.

[slideleft]

Thanks everyone for your interest.
I am providing another view of part from other side to better illustrate radius on sides. I cannot do this with 2D contouring (unless I did MULTIPLE layers). This is the largest of several small parts and is about .75" across, .25" tall. Using 3D contouring it is really easy for me to generate perfect toolpaths on side walls (.005" steps using a 1/8" ball endmill). The smaller nooks will be radiused with a 1/16" ball endmill. Filing is not an option.
Again, the part I can't figure out is- is there a setting with 3D contouring that will recognize and create toolpaths on the flat regions of a part? Why not? What is the next easiest way (I have a lot of designs with this issue- round stuff and flat stuff).
Thanks again.
Jeff
Mastercam X

[slideleft]

[inkydo69]

I suggest before you start, place on separate levels, the solid, the surfaces-created from that solid, and curves-created from that solid.
and not to modify these in any way. Don't create curves from surfaces if you can ( double ups, trim errors etc quickly appear )

If you need to create extra geometry, copy onto a new level and then modify/add geom and also name it accordingly.


It's like Superman said.... Create some extra geometry And just add some 2D contours to the program to finish the flat areas. Why would you want to run a 3D tool path if you don't have to? As fare as cutting on the Flats with a 3D tool path i am not sure there is a way without creating a new tool path. So why not just make it simple and cut them with a flat endmill.

Note .. We do not know how you think this part should be done, All we see is it would be just simpler to finish with a new 2d contour rather then a 3d. Just leave .005 on Z and add finish it.

Hope i made some sense it is 3am :tired:

[AlphaD]

First of all, good to see you all.
I am new on this forum, so please be a litle understanding with me. I have started to use mastercam 2 weeks ago , and I have managed to create a few programms that are working good. I need an advice. I want to check some previous programms, for wich I have the .nc file .How can I convert this programms in .nci files?

[Superman]

First of all, good to see you all.
I am new on this forum, so please be a litle understanding with me. I have started to use mastercam 2 weeks ago , and I have managed to create a few programms that are working good. I need an advice. I want to check some previous programms, for wich I have the .nc file .How can I convert this programms in .nci files?

1st---welcome to the forum

just to get it right.
you currently have NC code that has been run on CNC
and
you wish to get it back into Mastercam as geometry

What is required is a "Reverse Post",( sort of reads the G0-G3 codes only )

1. a little intuition is required when performing this, as knowledge of the actual code is needed (eg paths written as tool centreline or to the profile [wear, control comp used ], tools used, what strategy was used to create the toolpath etc).
2. this will only create 2D geometry ( lines and arcs only ) usually at the Z level it was machined at. You still have to manipulate the geometry to get the correct shape or profile.
3. this will not recreate a solid or surfaces
4. this will not recreate the operations that Mastercam would use to generate the actual toolpaths.

IMO seeing you have to do the last point above, it may be quicker to start fresh, you have the speeds / feeds / DOC etc, and quite often doing it a 2nd time you can be more efficient in your programming strategies

[AlphaD]

Thanks for the answer. I was thinking to import the code generated with .nc file into .nci file , because in X3 you can generate toolpath using .nci files. That's why I wanted this information.
Is possible to simulate a program by writing directly instructions like in .nc files ? ex:
"N160 G2 X-148.424 Y7.973 I-84.419 J-967.922 F1000.00 (F600)
N162 G1 X-148.361 Y-2.19
N164 G3 X-170.967 Y-3.541 I-17.539 J-2381.191
N166 G1 X-172.008 Y-11.626
N168 G2 X-136.314 Y-9.569 I-17.539 J-2381.191
N170 G1 X-136.478 Y16.695
N172 G3 X-170.641 Y14.293 I-84.419 J-967.922"

[cadcam]

Is possible to simulate a program by writing directly instructions like in .nc files ?

Sorry you can not reverse the code. I see you are writing in Metric. hence you living in the UK.