[Julian M]

The attached file is a casting for which im trying to use surface toolpaths to machine the face which is 2mm down from the outside face, which has the 5.5mm slot through it, the surface is green(not the recess around the open face) I have tried using high speed horizontal toolpath with little success. Any help would be gratefully received

Thanks Julian

[Matt Berube]

In my opinion the easiest way to put a toolpath on that face is just simple 2-d pocket.

1. switch to a color that has not been used yet.
2. create curves all edges of the face you are cutting
3. Select the pocket toolpath
4. when you get to the chain manager, use window mode and also turn on the color mask to whatever you set in step 1 then draw a window over the whole part. Chaining done !

This generates a toolpath very quickly.

Now if you really want to use the horizontal area why don't you post a Mastercam .Z2G file with your machine definition and tool library already loaded in the file and make your best attempt at the horizontal toolpath. From there it should be easy to redirect you.

When you did try it did you use depth limits ? You have to remember that that toolpath will automatically try to cut every flat area on your part unless you find a way to restrict it.

[ObrienDave]

Try something like these toolpaths as an example.

Remember, If you do NOT want a cutter to cut something or go somewhere, you have to either,

1. Fill holes with surfaces,
2. Restrict the toolpath with boundries,
3. Limit the depth of the cut with co-ordinates,
4. Any combination of the above restrictions or ALL of them.

ANY programming system can NOT think for you.
Programming systems can NOT read your mind.
You MUST learn how to make it work the way YOU want it to.
It is just like any tool in your toolbox, YOU must learn how to use the tool.
A tool is only as good as the person using it.

I apologize if this seems to be a rant, but, I run into this situation often.

[Julian M]

Try something like these toolpaths as an example.

Remember, If you do NOT want a cutter to cut something or go somewhere, you have to either,

1. Fill holes with surfaces,
2. Restrict the toolpath with boundries,
3. Limit the depth of the cut with co-ordinates,
4. Any combination of the above restrictions or ALL of them.

ANY programming system can NOT think for you.
Programming systems can NOT read your mind.
You MUST learn how to make it work the way YOU want it to.
It is just like any tool in your toolbox, YOU must learn how to use the tool.
A tool is only as good as the person using it.

I apologize if this seems to be a rant, but, I run into this situation often.

Thanks for this i really appreciate the help. I have managed to recreated for myself the 2d pocket toolpath but so far am unable to do the same with the surface toolpath. The problem i am having is creating the two red surfaces, i go create-surface-fill holes with surfaces, which seems to create a surface I also i set the max and min cut depths to -2mm but the toolpath still violates them. What am i doing wrong? why does it machine through the surfaces?

[Matt Berube]

why does it machine through the surfaces?

Mastercam will never violate a surface that is selected as drive or check. If it is not selected as drive or check Mastercam ignores it completely.

I suspect you do not have enough surfaces selected as drive. The safest way to machine is to select ALL SURFACES as drive and then restrict the toolpath with one or more of the options Obriendave suggested.

If this does not help I'll need to take a look at your toolpath.

[Julian M]

Mastercam will never violate a surface that is selected as drive or check. If it is not selected as drive or check Mastercam ignores it completely.

I suspect you do not have enough surfaces selected as drive. The safest way to machine is to select ALL SURFACES as drive and then restrict the toolpath with one or more of the options Obriendave suggested.

If this does not help I'll need to take a look at your toolpath.

Your a genius what would i do without your help. I created the surfaces but forgot to reselect drive surfaces, doh!!

Thanks again, julian

[cadcam]

Julian waht version of Mastercam X are you running as I went back with your first stament toolpath but I did it in X2 I can do it in an earler option if you let me know which one you are running so I can post it here.

[ObrienDave]

Julian,

One of the hardest concepts to learn, is to give Mcam just enough geometry to do the cut.
This makes for the fastest cut evaluation.
Why take a lot of time to do a surface cut if you can accomplish the same thing with a 2D cut?

The first computer I ran Mcam 6 on, was a 486-DX2 66Mhz, I think, about 15 years ago.
Compared to computers today, it was !@#$%^ *&^%$#@ slow.
I learned to only give it what was required.

You don't need surfaces that are under the part.
You don't need vertical surfaces as long as you use, under the advanced button, roll tool around all edges or define the tool long enough so it can not fit UNDER a surface.
You only need surfaces that would be "seen" by the spindle or come in contact with the tool.

I may be in error about the under part, and, I know other programmers will have different techniques to deal with evaluation time.
The point being, better safe than crashing.

I deal with molds that range from a few inches big to about twice the volume of your average bathtub.
From a few surfaces to literally, tens of thousands.
I do not want Mcam to take HOURS to evaluate a toolpath even with a 2.4 Ghz computer.

Check it out.
http://www.ecscase.com/

Remember the KISS principal.
Keep It Simple, Silly!

Good luck and keep plugging away at it.

Matt,

Thanks for your help.
I had to work today, so I am a little slow on the response.
I always enjoy your suggestions to the "newbies".

[Julian M]

Julian waht version of Mastercam X are you running as I went back with your first stament toolpath but I did it in X2 I can do it in an earler option if you let me know which one you are running so I can post it here.

Hi cadcam i am running MC-X MR2.

Cheers julian

[Matt Berube]

The point being, better safe than crashing.

For me, that is the golden rule. I try to err on the side of caution.

It is a real momentum killer when things take too long to regenerate though.

My favorite new 'style' of working is not to use surfaces at all. I model up my part in solid and select "drive" in one click (X2). I love that.

In the past week I made around 30 electrodes and I think I used surfaces in 2 of them. The rest were solids.

[cadcam]

Julin here it is in MCX-mr2, MR2 does not support check surfaces so a tade diffrent in X2

[Julian M]

Thanks all of you for helping me with this i am finally starting to get the hang of it! Although i have another question, how do i modify the size of a fillet between two surfaces for instance the fillet connecting a boss to a face?

[Matt Berube]

Julian, do you have solids ?

[ObrienDave]

Julian,

Unfortunately, you can not modify a fillet SURFACE.
You can copy, translate, offset, extend the edges, and a few other things to most types of surfaces.
You can not modify the curvature of an existing surface except for scaling.

You can, however, make a new fillet surface over the top of another one.
In Mcam9, Create surface, fillet, plane/surf or curve/surf or surf/surf, whatever the case may be.
I do not recommend using the trim surfaces option because I prefer to keep as much of the ORIGINAL geometry as possible.
This way some engineer can not say you destroyed HIS part.
But that is another rant for another day.

You may have to change the NORMAL of the surface to get the fillet on the proper side.

Please review the attached ZIP file.

Please remember to re-select drive surfaces.

If you have the solids option, an easier way to do it is to make a solid of your part.
Not from surfaces, but from scratch.
This way you have the, for lack of a better term, "history" of the solid construction.
This makes it REALLY easy to modify just about anything in the model.

In my opinion, Mcam solids is a subset of SolidWorks.
Mcam solids will do about 20% of what SolidWorks can.
If the solids manager shows ONLY a body, then it is impossible to modify EXISTING fillets.
You can ADD operations to the solid such as, holes, add bosses, put new fillets at SHARP corner intersections, but, you can not modify EXISTING fillets because the solid is ONE body.
Anything YOU add to the solid can be modified.
If you are not familiar with creating solids, the easiest way to learn solids is to do it just like you would machine it.
Start with a solid block and cut it using geometry.
Of course, there are easier ways to create complex solids.
But start with ways that are familiar to you.

Attached is a solid of your part without all of the IGES junk.

Matt,
Here is my opinion on surface machining solids from an earlier, pre McamX, thread.
http://www.cnczone.com/forums/showth...4812#post74812

[Julian M]

Julian, do you have solids ?

Matt, i only have this part in iges format, i do however have solids option.

[Julian M]

Julian,
You can, however, make a new filet surface over the top of another one.

Dave, how would i do this if i wanted to create a 5mm fillet over a 3mm fillet?
Thanks Julian

[ObrienDave]

Julian,

Please re-read the above message.
I was in the middle of editing.
TTFN

[Julian M]

Dave,

Been very busy over christmas and forgot to thank you for all your help with
this i appreciate it.

[ObrienDave]

Your quite welcome.
Glad to be of help.