Need quick help in X2MR2

[bob1112]

We are trying to use another shop's software to program this part in X2MR2 and simply cannot get it to do what we want. Wondering if anyone would be willing to look at the part and sample program a certain surface? We do not get much seat time so we need to go in prepared. I have an IGS file and will email it to someone that can help. Just need to know what function to use. We are trying to use a contour path and it runs the outside perimeter of the cut but not the inside. Probably will make more sense with a part pic but of course I cannot upload much here.

OK, I got a pic loaded. Basically, we need to program the "toilet seat" area of this part with a 3/8 EM. If we select that stepped down surface with a contour path, it will simply run the outside of the line. We simply need to enter from the side and hog off that stepped down ring area. What are we missing? I would prefer to drive right through the center of this area in one pass. we need to leave the center high or untouched so we can flip the part and then run the inner profile from that second position.

[Derek Goodwin]

here's one way to do it, quick video, no sound

click on the link that says offset contour

http://eapprentice.net/index.php?opt...d=53&Itemid=75

Mastercam training Online http://eapprentice.net/

[bob1112]

Thanks, I am simply not familiar enough with MCX and have never used the surface paths. As I understand it, the drive geometry is what will be cut, the check geometry is what gets left, when I attempt to program the surface contour path, I get an error that both check and drive geometry are identical even though I have selected different geometry for both. Any idea what I might be doing wrong?

IE, for check, do I select all surfaces that are not drive geometry or just on one plane? Just trying to get past this identical geometry error at this point.

[dpark1]

Post an IGES file if you have one.

[Derek Goodwin]

the example I gave you is for a 2D toolpath. if that surface is curved it would require 3D toolpath, flowline would probably be a better option than surface finish contour. (Contour is better for surfaces that are closer to vertical than horizontal) drive surface is the surface you cut, check surface is the surface to avoid. The error that drive and check surfaces are the same, usually occurs when you select a solid body, in that case you can click OK and ignore the error, the toolpath will work fine. The important thing is to have a strategy for making the part: work holding, roughing, finishing and the subsequent operations. Its more than just picking a toolpath, as dpark mentioned, post up a file and somebody will help.

Mastercam training Online http://eapprentice.net/

[bob1112]

Believe me, I have a complete part in my head and having blanks cut right now. I have to drill the center of that ring and put a SHCS for later fixuring so I cannot remove the center right now. Just need to face that stepped down surface efficiently.


How do you guys import and prep your file to put tool paths on? What file type do you use? I understand maybe stp files are a good option...

[cadcam]

Send me you MC file.

[mastercamguru]

I took the time to convert your surface model to a wireframe for you and found multiple splines overlaid. Often engineers don't clean up their drawings and sometimes files don't convert cleanly into Mastercam. That creates chaining problems if you don't analyze your geometry first. I created lines and arcs to replace your surface edges and left the sloped surfaces for 3-d toolpath on the other side of the part. Generally speaking it is much easier to just delete the surfaces and toolpath standard geometry(lines and arcs) rather than surface geometry for 2-d toolpaths. Check your e-mail for the MC9 file. MCX/MCX2 will open it just fine. I think you will find it much easier to toolpath efficiently.

[bob1112]

Guru, you straight up nailed that path I was looking for!! Thanks so much. At least now I know we can create the path we want, I am still just a bit lost. Are saying in order to program this part, we need to create lines and arc everywhere but that ramped area that will require 3D contouring? Can these problems be solved with a better file for import? Something maybe we can do in our CAD model before we save it?


I guess I am just trying to streamline the process for a part like this and learn what we need to do. How the heck do you selectively create lines and arcs and still leave that ramp 3D? Is there no way to create tool paths like you did with the 3D paths?

Thanks so much for taking time to look at this. I know we are wasting some time here but I am trying use this example as a learning tool right now. We have someone willing to let us use their software so we want to be proficient with it.


Edit: I noticed you added some lines to get those paths on the part. Will we have to do this? Is there no other way?

[cadcam]

Originally Posted by degmc here's one way to do it, quick video, no sound click on the link that says offset contour http://eapprentice.net/index.php?opt...d=53&Itemid=75 Mastercam training Online http://eapprentice.net/

I would like all to also review my video covering the same well almost the same options. This just to give you other options for the same thing.
http://www.mastercam-cadcam.com/vide...toursample.htm

[cadcam]

Viper please review the paths and the geo used for the paths I created from Mastercam Guru.

you will notice I did not make extra geo for pathing but used the exit main wire he created. I also never turned off the cutter comp so now you have cutter comp for both paths.
and also minimized the cut time not running the cut across the entire back wall.

Just showing there are more ways and more power in the system then most know of.
this is a X2 MR2 file.

I will also posting on more thoughts of how to get what is needed from your file.
I have not seen the first file. is it an Iges or a solid file. this all makes a diffrence on how you handle the files as they come in.
If possiable I would like to see the file from the customer?

[bob1112]

Our customer only supplied a drawing so we have to create the CAD file. It was saved as in IGES file but we can save as about anything if we know what MCX prefers to work with. We had just understood in the past that the IGES file was preferred for MCX. I will take a peek at your file tomorrow to see what you have done differently. I will say, it was my intent to cut all the way across the back to relieve it so when I cut that ramp from the other side, most of the material will be gone.