Open Pocket, why isnt this easier?

[slougee]

New MC user on the 2017 interface. Coming from 5 years as an Esprit user. I have a SIMPLE part with a open pocket, and varying levels. The 3 day training program was not as toolpath oriented as I thought it should be and focused on alot of drawing. NOW, working with a solid model I SHOULDNT have to creating wireframing everywhere on a simple part to get what I want. I feel this is doubling the amount of work to achieve a result that should be easy. I am used to some level of pocket recognition, or  could create chains and modify which were open and which were closed. I can KINDA do the same thing on this part in MC, but I DO NOT want to dynamic machine anything. I know MC is hard up on the dynamic machining, which is GREAT, but this is a simple aluminum part that does not require it. Im sure alot of this venting is being new to the software, but being new, something this simple SHOULD be simple to a new user.

 

 

[Gracjan aka Pullo]

1. draw a wireframe  rectangle which is slightly larger than the part .

2. rough it out with a pocket rough (using this wireframe rectangle)

3.  use the contour finishing , with flats turned on to finish the verticals walls and the floors

4. You have something small there which is not visible so a fourth and fifth op is warranted . 

 

Should take about 5-10 minutes of programming by the time you get good at this.

 

Gracjan

[Colin Gilchrist]

You will, at a minimum, need to create a Tool Containment Boundary. Just a simple Rectangle. Place it in "Z" wherever you Material "starts". This is to keep the tool from cutting on the "outside" of the part, where you probably have it held in a Vise, and machining there would not be good.

 

Then use a "3D Pocketing Routine". There are several different tool paths available in Mastercam that would make short work of this. I have no idea why you wouldn't want to use the "Dynamic" paths, since they are much more efficient that a normal pocketing routine, but that's up to you.

 

Right Click in the Operations Manager > Mill Tool paths > Surface Rough > Pocket. Choose your solid, and select your Containment Boundary.

 

In the Tool Path Parameters, make sure that "Inside" is set for your containment boundary, and it should cut the whole shape in one path.

[slougee]

Dynamic for something is this will create alot of air cutting. The tool in this case doesnt need to be optimized. It can slot all day long without the need to smooth the toolpath.

[slougee]

Colin, Doing as you described still plunges the tool into the edge of the material. It does get me a better toolpath however.

 

NOW with basic pocketing, how can I simply select a rectangle, tell it which edges are open, and pocket that rectangle? No other boundary wires frames, just one simple open ended pocket. I dont even need multiple depths. I will just create another pocket for another depth.

 

Just one double open ended pocket at one Z level. Thats it

[mikenaturalice]

Colin, Doing as you described still plunges the tool into the edge of the material. It does get me a better toolpath however.

 

NOW with basic pocketing, how can I simply select a rectangle, tell it which edges are open, and pocket that rectangle? No other boundary wires frames, just one simple open ended pocket. I dont even need multiple depths. I will just create another pocket for another depth.

 

Just one double open ended pocket at one Z level. Thats it

I don't have much advice, except if you are dead set on doing it how you did it in Esprit you are going to have a hard time at it. 

 

Can't tell how big your part is, but... If you import the model with edge curves all you would need to do is extend the lines the same as your tool diameter and then close them up, now you have a boundary at every level. Lots of ways to make this part, none of them being hard, or requiring much work IMO.

[Jayson Kramer]

Here is a a simple open pocket paths with wire and solid. hope this helps.

open pocket.zip

[slougee]

Hi Jay, still wasnt quite what Im looking for due to the tool not actually exiting the material on the opp side of entry. 

 

I ended up just extending the lines, making it a closed pocket, and that clearance from the extensions was enough for the tool to enter and exit.

 

[Jayson Kramer]

Hi Jay, still wasnt quite what Im looking for due to the tool not actually exiting the material on the opp side of entry. 

 

I ended up just extending the lines, making it a closed pocket, and that clearance from the extensions was enough for the tool to enter and exit.

in the case you could of just did a contour and been done. there are other ways to do this but you stated not using any of the dynamic paths not sure why. then you could defines the ends as Air regions. but I am glad you go more of what you wanted.

 

regards and welcome to the Mastercam side.

[slougee]

I thought of using a contour, but say the pocket were much wider. I would have to create likely 2 contour operations for one pocket. Again, I may just be too new to the software. As for dynamic, on deep pockets where full LOC tool engagement, or tough materials, its extremely useful. I just dont see the use for it on easier to machine materials, and lower cutting depths its just not practical (feature based of course)

[Jayson Kramer]

Now here is the same file I posted earlier with FBM Mill look at the path motion and it took 30 seconds to program.

open pocket FBM.zip

[jlw™]

I don't have much advice, except if you are dead set on doing it how you did it in Esprit you are going to have a hard time at it. 

 

Can't tell how big your part is, but... If you import the model with edge curves all you would need to do is extend the lines the same as your tool diameter and then close them up, now you have a boundary at every level. Lots of ways to make this part, none of them being hard, or requiring much work IMO.

 

 

As a former Esprit user myself, I assure you once you give up on doing it like Esprit and do it like Mastercam you will have a better day.  Email me if you would like some tips on transitioning from Esprit to mcam.

[JoshC]

There are multiple solutions here, 3D toolpaths are probably fastest but i would probably just go 2d on that part as long as those are flat. Then i would narrow it down to two choices, Either 2D Dynamic or 2D Area mill. Either solution uses the same chaining methods, which in that case would be pick the rectangluar floor for the machining regeon and then pick the areas that the tool can not go using the Avoidance area, toolpath would be then set to "Outside".

Chaining:

​

Results:

​

 

Like I mentioned this is just 1 approach and there are other solutions that would work really well too

[jlw™]

I'd create 6 lines in the corners and use 2d contour and be done in one unit of it doesn't need rough and finish.

[MrFish]

Similar to JoshC but I would use 3D area clearance, just choose the faces you want to machine, set to outside approach and push go. Simple toolpath with over runs at each end and 3o seconds to program straight from the solid with no extra wireframe geo needed.

temp.mcx-9

[goooose]

Without opening a huge can of Esprit vs Mastercam....

 

Mastercam really needs to up its game on toolpath creation from solids. Nobody wants to draw additional geometry just to get a toolpath outside of an 'open' edge. CAM software should be able to do this, and Esprit does (I'm sure there are others that do as well). 

 

That being said though, could you not just use a 2D HST so you get the good chaining options but use an area mill path?

[absolute technologies]

Without opening a huge can of Esprit vs Mastercam....

 

Nobody wants to draw additional geometry just to get a toolpath outside of an 'open' edge.

I guess I'm a nobody, I prefer to draw my own geometry to dictate the toolpath the way it needs to be not the way MasterCam decides it wants to create it, it's called control, but then again I'm old school. For me it's not about how fast I can create code but rather getting the technique proper and not wasting time at the machine. If I spend a little extra time in the CAM system it doesn't cost the company hardly anything in comparison to wasting time at the machine with some program that took only 30 minutes to create. But then again I don't work for a mom & pop where the owner is looking over my shoulder constantly so I understand many guys are programming parts they'll never see again where it's more important to just crank it out. I do know though there are a lot of programmers out there that are either lazy of just don't know cutting strategy and have to take what the CAM system gives them.

 

We had a couple of parts that we farmed out to an experienced programmer that used all these new school paths. Out of the box it was 16 hours cycle time and after weeks of trying to get it to run we finally got to do a little optimization and got it like 9 hours. After reprogramming with proven strategies it was under 3 hours. With our current orders it was close to 1,000 hours savings for the machining,  for each part! Other than just a bad cutting strategy in general the biggest factor in the savings was a 6 meg file vs 300K and the fact that the large file cut air most of the time repositioning itself for the next cut. I found it interesting that the large file only had only a couple of minutes of rapid time where the more efficient program had like 10 minutes of rapids. A 300k file will execute much faster than 6 meg file..

 

IMHO, other than Mill/Turn and doing some edge breaks, Esprit blows donkeys in comparison.

 

Cheers!

Len Dye

[Newbeeee™]

.....blows donkeys in comparison.

 

Cheers!

Len Dye

Never heard that expression before

[goooose]

 

 

IMHO, other than Mill/Turn and doing some edge breaks, Esprit blows donkeys in comparison.

 

Cheers!

Len Dye

 

 

I think OP was looking for solutions for open pocketing...not how awesome you are at wireframe programming.

[Colin Gilchrist]

Mastercam does need to step up it's game with true "Material Tracking". A Stock Model is an "after the fact" solution, most of the time. Many CAM software packages do a better job of Machining from a Solid Model, and managing "Stock material" through the machining process.

 

Personally, I'm with most of the guys on there though; I like using Wire Frame geometry for the control it gives me over the machining process.

[Jayson Kramer]

^^^^^

Who the fvck are you?  The forum police???

No thats my job . lol

[#Rekd™]

+1 to Colin on the wireframe and having more control!

[Newbeeee™]

No thats my job . lol

Iv'e always wondered what your job was

[Thee Rickster ™]

Iv'e always wondered what your job was

its not a job, its a lifestyle!

[Thad]

its not a job, its a lifestyle!

 

Great! I suppose next you're gonna want your own bathroom?