X2 Machine from Stock

This May be taken care of in a later release, but im stuck with X2 for now. I also use FeatureCam regularly, and I love it. A great benefit from it is the ease to machine from stock. FC recognizes stock, and will generate code to machine a given contour, and all the existing stock around it. Even when I create a bounding box, with stock and /or solid I can tseem to get it to machine everything else. MC just cuts around the contour and thats it. Especially with surface milling. Makes roughing very difficult.

Any help will be appreciated. thank you.

Is this a question? Or are you a Troll? Roughing with MC is SIMPLE.

Yes it is a question, And what if I am a troll? Do you have something against them??

HAHA ok.

So what is the question? You need to tell us where you are stuck. Sounds like you don't know the software at all.

I know my way around it well.I have just never tried it before. I have a simple boss profile, that I want to machine from a large piece of stock. I want to machine it from the outside -in, and rough away all the stock. Not just go around the profile. make sense?

The simple answer is just use multiple paths on a single contour. Add enough passes to compensate for the amount of removal per side and you are done.

So, if you have 1" of stock to remove on a contour (per side) and you take a .25" cut, just put 4 rough passes at .25" per pass. Comprendo?

Super quick, super simple.

Quote:

---

Originally Posted by WallyL7

The simple answer is just use multiple paths on a single contour. Add enough passes to compensate for the amount of removal per side and you are done.

So, if you have 1" of stock to remove on a contour (per side) and you take a .25" cut, just put 4 rough passes at .25" per pass. Comprendo?

Super quick, super simple.

---

Ive done that plenty of times. I was just hoping for something a little more efficient. If the contour doesnt have the same shape as the stock, it tends to cut a lot of air.

What MC release did they start their feature based machining? I have that on Featurecam, and it is great at reducing program generation times, and makes efficient toolpaths.

Unfortunately, X2 does not have allot of options for 2d roughing. You would either have to create extra geometry to get an efficient 2d roughing tool path or accept that you are going to have an inefficient path that is easy to create.

The feature base machining in mastercam is a joke at this point. It works but not well enough to rely on. BUT! there are several 2d roughing operations added since X3 that are far more efficient than what you are using now. X6 will be even better rumor has it.

If you are stuck with X2 unfortunately you are going to be stuck having to create geometry to drive your tool paths if you are looking for efficiency.

use pocket facing option pick you main boundry and then the inside profile. make sure to set enough overlap to cut all edeges of the stock.

set for outside to inside and have it not finish main boundry so it will only finish the standing core area.. this option is real old.

let me know if you need a sample,

Good call cadcam. Mastercam gives so many options that I've never had any trouble getting it to do what I want - and since MC is so easy to draw in, it normally only takes seconds to get a stock profile defined. Unfortunately, though, it seems MC lathe has the better stock recognition features. Seems they are working on it for MILL so hopefully we will see something there soon.

To the OP - why don't you just stick with Featurecam if you are so happy?

Quote:

---

Originally Posted by cadcam

use pocket facing option pick you main boundry and then the inside profile. make sure to set enough overlap to cut all edeges of the stock.

set for outside to inside and have it not finish main boundry so it will only finish the standing core area.. this option is real old.

let me know if you need a sample,

---

That option is only practical in SOME situations. If you do not want your cutter charging in to material and burying itself then it can be hit or miss.

Quote:

---

Originally Posted by cadcam

use pocket facing option pick you main boundry and then the inside profile. make sure to set enough overlap to cut all edeges of the stock.

set for outside to inside and have it not finish main boundry so it will only finish the standing core area.. this option is real old.

let me know if you need a sample,

---

Thats it!! Thank you. Very easy to do. Ive seen that option there before, but never thought to try it.

Quote:

---

Originally Posted by WallyL7

Good call cadcam. Mastercam gives so many options that I've never had any trouble getting it to do what I want - and since MC is so easy to draw in, it normally only takes seconds to get a stock profile defined. Unfortunately, though, it seems MC lathe has the better stock recognition features. Seems they are working on it for MILL so hopefully we will see something there soon.

To the OP - why don't you just stick with Featurecam if you are so happy?

---

Ive been a long time MC user, and the last 3 years ive been on FC. I just want to try and get the most from MC as well. I tinker around with designing in my spare time, and machining on the side. I dont have FC available to me as much. Believe me, FC isnt the best at some things. Its great for Programming, and Gouge checking, and surfmilling. But inefficient at drafting, and we dont have the modeling package with it. So I cant develope any 3D models. We use both here, but they each have their strengths.

Quote:

---

Originally Posted by neurosis

That option is only practical in SOME situations. If you do not want your cutter charging in to material and burying itself then it can be hit or miss.

---

I have not had that issue you speak of but I guess some were this can be an issue. but if you Morph cut for example this will not be an issue.

All option have there good and bad applications.

I can show you several examples of this including using morph (which is a horribly inefficient tool path to begin with).

Granted, its been a while since ive had to use this function at all since we now have much better roughing paths to work with.

This was always a pet peeve of mine in versions of MC prior to X4 (x3 actually which I refused to use). Too much geometry creation to get efficient tool path that would actually work without destroying cutters. Now obviously this depends on your machining technique and how you choose to remove material but I do not like to change my machining techniques to suite the system. It should be the other way around yes?

I can give you several examples of this if you would like to see them. If your diameter or feature is close to the same size as your stock then it never becomes an issue BUT of you have a feature or features that are inside of your stock boundary that have distances from your stock edge greater than your cutter diameter, it will channel to location and then work its way around to remove the material. This includes the morph pocketing path.

I agree about not having to Tailor your likes to the system. All of them should have the ability to adapt to your needs.

With that said, I have had some time to play with the feature. I constructed 2 rectangles, and a circle, all inside a larger rectangle. And found the morph toolpath, generated a LOT of redundant cuts. Most were re cuts of very little stepover. The parrallel Spiral and constant stepover were the least amount of code and redundancy. While its not Ideal, but still a really good option when avoiding creating extra geometry.

Thanks for all the help in the matter. much appreciated.

I think that if a majority of your work is aluminum then the path would probably work fine for the most part. We machine mostly hard metals here so

1. Conventional cutting is out of the question in MOST cases

2. burying the cutter in material/channeling is out of the question in MOST cases

Even attempting to use insertable tools with this method in hard metals can prove to be hell on inserts/tool life.

You may have some luck with high feed mills but I would not use this path even for that application.

Generally, once you are familiar with the system, the construction geometry needed to create efficient workable tool path does not take that long. Back in the pre-X4 days I would determine my plan of attack before ever creating a single path. I would then start creating construction geometry where ever I though it necessary and place that geometry on labeled levels.

With the available paths in current versions I have to create very little construction geometry. The "Dynamic" tool paths are the golden ticket!

I found that out too! I can create needed geometry pretty quick, And Most of my stuff is Aluminum. I have been using for years now, but just took a Hiatus for a couple years with FC. Just by offsetting my original chain, to the desired stepover i want, adn trimming back the rest is quick. It just creates a lot of seperate tool paths. Such is life right!

I know a couple of people that use FC. They love the software.