[SRT Mike]

I am trying to learn Mastercam X3 and get productive with it as quickly as I can. I was sort of thrown into this job last minute without warning and I need to get a couple of parts done asap I am starting with the most complex one.

See attached picture. Basically a rectangular piece of aluminum, with rounded ends. There is a shelf 1/8" down from the top, then there is a pocket 1/4" deep. Then there are three cut-outs (with 1/8" corner radii), 7 holes, and 2 "bosses" that stick up and get drilled/tapped. Then there are 5 pockets that are 0.050" deep.

I imported the part into X3 and set the work coordinate system to the top face as shown.

First problem is when I try to pick a facing operation and select the top surface, it says "facing does not support islands, use pocket facing". I dont understand why - I don't see any island? The bosses are 1/8" below the top surface, so why can't I do a facing operation on the whole top?

Second problem is when I try to create a pocketing operation, and I select the bottom of the cavity and select, say, a 1/4" flat end mill, the toolpath it creates only goes in the open areas where a 1/4" EM will fit... it doesn't do the whole bottom surface (even though it could pocket it all to that depth since the pockets that go straight through are obviously deeper than the bottom face). I want it to pocket the whole base to that level... then I wanted to make a 2nd pocketing operation to cut out the straight-through rectangles, then make a 3rd pocketing operation to cut the five 0.050" deep pockets. But it isn't working that way.

I did see a tutorial that talked about placing a temporary surface over holes to "cap" them so that a toolbit wouldn't try to go into them, but that's not happenning here... the toolbit is just avoiding the areas entirely.

I was able to get the pocket made with a "surface rough pocket" toolpath, but this has 2 problems... first, it does finish passes on each stepdown in the Z axis, whereas I would prefer to do a finish pass at the very end at full depth (and I dont see any option to change this). The second problem is that the three pockets that go straight through, it machines them down to the very bottom of the stock, but I don't need that... I will be machining the other side, and so I only need to go a hair over 1/8" below the bottom of the pocket (just break through a little) and with "surface rough pocket" I don't see any option to only pocket down to a specific depth, it seems to go all the way.

Any tips are greatly appreciated!

[Superman]

We'll see what we can do
Question 1: What experience are you at with Mcam ? ( lets us know how simple / complex we give the answers ). You sound like a early Mcam guy.

Problem 1
If you have stock drawn, then your 1st facing can use the "stock geometry",
to select this method, don't select any geometry at all.
If just a single pass is what you need, create a line down the centre that overhangs the stock by 60% of the cutter dia, select 2D contour and this line you've drawn, with comp "OFF" ( there are lots of tricks and methods to do what you need, any method is good as long as it is quick and dosen't stuff to part or tool )

Problem 2
You only said pocket, what type 2D / surface / HSM ?
If 2D, select the contour that defines the pocket walls and go from there
If "surface pocket", select the surfaces that make up the pocket as "drive surfaces" ( walls, floor, fillets ) and anything you don't want the tool near as "check surfaces"

I did see a tutorial that talked about placing a temporary surface over holes to "cap" them so that a toolbit wouldn't try to go into them, but that's not happenning here... the toolbit is just avoiding the areas entirely.

2 methods - "Remove Boundary" ( removes the hole/s completely) and "Fill Holes" ( creates a surface patch to cover the hole/s )

This job seems like all 2D strategies, what about fillets ? using bullnose cutters ? cutters with small radii tend to leave floors smoother and not create lines around the walls.

Surface toolpaths are a little awkward to explain, each strategy can have multiple outcomes by altering a different parameter each time and the settings now, may not be suitable for a different shape next time.
Whenever using surface toolpaths, try selecting the bare minimum and add in the other bits when required.

Hear from you soon
Steve
PS: I have X2 ( no real change as to where the icons etc are as in X3)

[kesparate]

is it allowed on the forum to post the model? given a tool list (ideally tools in the default library) and the model i could knock this up in a few minutes and you could just see the strategies used and the settings.
i suspect that this would be the easiest way to learn a bit really quickly. though, i've been going to the official training classes from my reseller, and i'm telling you this program is complicated. i bet there's crap that can be done that even guys with years of experience would find surprising.
that's why i love it when sales guys bring in other cam systems and explain how you can learn them in a week. that can only mean one of two things....

[SRT Mike]

Thanks for the feedback guys.

Superman,

On my experience with X3, I would say I am very much a beginner. I just started a couple of weeks ago. We had a guy here that used to do it but he is only working here a day a month or so and to be honest he isn't as much into training me as he is into "just give it to me and I'll do it". Thats great but I need to learn it myself, so I can do it on my own I do the 3D design in Solidworks and I program the machines (until now I've done it manually) and I did play around with Visual Mill some years ago... so I know the concepts of CAM and machining, but I dont know MCAM X3 really at all

Thanks for the tip on selecting the walls of the pocket... thats probably what I was doing wrong. I was selecting the base as a face. I'm surprised the program isn't "smarter" to know things like that it can machine over a surface, even though there is a feature there, because the feature is below the machining surface.

I checked out a tutorial video on FBM mill toolpath... it looked great, like a one-step way to machine a part. I diligently followed the instructions, and it created a bunch of toolpaths that had errors So I figured I better figure it out on my own.

The pocket in question is actually 3 different levels of pockets... you can see in the attached image... there is the main pocket, then there is a 2nd set of pockets (the through holes) then a 3rd set (the 5 rounded rectangles). I wanted to have 3 pocketing ops... I think if I can do it by selecting the wall surfaces, I will be good to go. I'll give it a shot and see if it works.



kesperate,

that is a very generous offer, if I post the model in IGES format, would that let you open it in MCAM and do some paths? It is very kind of you to offer that, thank you! I agree this software isn't simple... I've been playing with settings and regenerating toolpaths to see what effect it has, and 90% of the time it doesnt have the effect I think it would

[tstom]

Mike,
It sounds to me like you are trying to do 2d machining by picking 3d entities(surfaces and solids) The prefered method in MC is to create boundary curves on your solids/surfaces and use them for the 2d toolpaths...no need to use surfacing toolpaths to do 2d work.....keep it simple...even with different depth islands it's still 2d work

if you post your part in .iges I can help you with it or for that matter I can open the Solidworks file

[SRT Mike]

Thank you tstom for your generous offer.

I have the file in IGES format on my desktop here, I think the updated solidworks model is at home, so I'm posting the IGES file here... my machining plan is to start with 1" thick stock (the part is 0.7" high). I wanted to face 0.050" off the top then cut the back first (the side with the round bosses), then cut the exterior curve also and go down to 0.800" deep (so I can go 0.050 below the bottom of the part, and have 0.150 to grip it in the vise). Then I want to flip it over and since the whole exterior will have been machined and I can just do the pocket in the front.

I appreciate your help - thanks!

[jharts1]

m'cam is not good sw for the massses, BOBcad out sells it 10 to 1.
my x3 never worked from the day i it put it on my system,so i can't use it if i wanted to if you over payed fro it, the local rep could hold your hand somemore, or your screwed, remember this sw is on ly marketed to
large companies,,, ,,

[kesparate]

ok so here are some initial tool paths. first off i notice that this iges file is all trimmed surfaces. i'm guessing this is whats giving you fits.
the easy way to handle this is to go to create/curve/curve on all edges
then window select the entire area and hit the green ball. now you will have geometry at all the edges of the surfaces which you can use to create tool paths.
next thing you should notice is that i have used different levels for all the tool paths. to create a new level click on the level button on the bottom of the screen and the level manager will pop up. there's a space to type a new number and a level name. this will create a new level.
to move geometry to a new level select it and then right click on level. it will give you a dialogue related to moving the geometry.

what i did was move the surfaces i was going to deal with to the level i wanted them on. then do the create curves thing.
then you just need to chain the geometry and add the details for the tool path. an important function for this is the join entities function under the edit menu.

if you don't understand chaining (as i didn't when i started mastercam as i came from esprite) then you're really at the beginning and you're probably going to need some hands on training.

please be aware this is really down and dirty tool pathing. just for sample purposes.

[SRT Mike]

ok so here are some initial tool paths. first off i notice that this iges file is all trimmed surfaces. i'm guessing this is whats giving you fits.
the easy way to handle this is to go to create/curve/curve on all edges
then window select the entire area and hit the green ball. now you will have geometry at all the edges of the surfaces which you can use to create tool paths.
next thing you should notice is that i have used different levels for all the tool paths. to create a new level click on the level button on the bottom of the screen and the level manager will pop up. there's a space to type a new number and a level name. this will create a new level.
to move geometry to a new level select it and then right click on level. it will give you a dialogue related to moving the geometry.

what i did was move the surfaces i was going to deal with to the level i wanted them on. then do the create curves thing.
then you just need to chain the geometry and add the details for the tool path. an important function for this is the join entities function under the edit menu.

if you don't understand chaining (as i didn't when i started mastercam as i came from esprite) then you're really at the beginning and you're probably going to need some hands on training.

please be aware this is really down and dirty tool pathing. just for sample purposes.

That makes perfect sense! Yes, I understand the concept of chaining, and the whole level thing makes perfect sense too. I am not sure if I was having problems with the details being trimmed surfaces because I was originally importing the Solidworks model. But after running the verify on your toolpath file it makes perfect sense.

Thanks, that helps a LOT! I think I can do the other straight-through pockets from here based on your help. I will do the drilling and tapping from the other side, so that I can just tap straight through.

Thanks again, I really appreciate your time!

[tstom]

Mike,
I programmed most of the bottom (side with bosses) It was like I thought ...you didn't have any 2d geometry I created most of it using "create curve one edge" then you use that as machining boundaries also if you place your curves correctly you can use the radio button in the tpath page to pick you top of stock and cut depths I didn't add any depth cuts but you can if you don't want cut cut some areas in one pass the button is also on the tpath page

If you create curves one edge and the toolpath faults saying boundary is not closed go back and use "trim 2 entities" some of the ones I did overlapped and I had to trim them Also on the small pockets in the bottom I had to manually draw the line to close the open end at the correct z height
there are many ways to machine parts in MC this is just one....but always start simple and work you way up ...2d then 3d etc.

let me know if you need more help I left the other side as "homework" for you


forgot to mention I only set the facing for -.025 If I have .050 to work with I usually like to face both sides to make sure the part is parallel

[SRT Mike]

Mike,
I programmed most of the bottom (side with bosses) It was like I thought ...you didn't have any 2d geometry I created most of it using "create curve one edge" then you use that as machining boundaries also if you place your curves correctly you can use the radio button in the tpath page to pick you top of stock and cut depths I didn't add any depth cuts but you can if you don't want cut cut some areas in one pass the button is also on the tpath page

If you create curves one edge and the toolpath faults saying boundary is not closed go back and use "trim 2 entities" some of the ones I did overlapped and I had to trim them Also on the small pockets in the bottom I had to manually draw the line to close the open end at the correct z height
there are many ways to machine parts in MC this is just one....but always start simple and work you way up ...2d then 3d etc.

let me know if you need more help I left the other side as "homework" for you


forgot to mention I only set the facing for -.025 If I have .050 to work with I usually like to face both sides to make sure the part is parallel

Thank you Tom! I checked the file and it makes sense what you wrote also... I am going to take a shot at the other side myself as soon as I get a few things done today I need to do

Thanks again - you guys helped me out HUGE!

[tstom]

m'cam is not good sw for the massses, BOBcad out sells it 10 to 1.
my x3 never worked from the day i it put it on my system,so i can't use it if i wanted to if you over payed fro it, the local rep could hold your hand somemore, or your screwed, remember this sw is on ly marketed to
large companies,,, ,,

I like to see the sales figures on that BobCadvs Mastercam statement and as far as MC not being for the masses that's just BS I'm a 2 man shop and I've been on since V9 My X3 works fine

[Superman]

For quick, good reference:

check your samples directory, various strategies and shapes, 3-axis thru to full 5-axis stuff, also should also has design files. these files usually go hand-in-hand with examples in the self-teach manuals

check-out the videos as well

As you can see, put your hand up for help, and it's not far away

CAM-on
Steve

[taqarth]

I personally would have made this part without any CAM, as it isnt a complex part, then carry on trying to learn Mastercam.

It is very hard to learn anything when under pressure to produce

Also very easy to get bogged down in the details when the customer just wants his parts lol.

[cadcam]

I would like to share my version of programing the part. this was all done with a solid model. just like if I had been given the Solid works file.
I have programed the hole part both sides. this is a MCX version 3 file.
Also there is a picture after verify. See if this helps.

[SRT Mike]

Well a big thanks to everyone who helped.

The tips here, along with signing up for streaming teacher, has definitely helped me out. I've been playing with Mastercam and am starting to get the hang of it, a bit anyway.

There is one issue I ran into today that I am hoping someone could give me a pointer on. See the attached images...

This is a fixture plate, and it has three 3.5" wide shelves with a 0.5" slot runnign down the middle of each shelf for some fixturing hardware. The raised outer edges have a chamfer, and there is 2 marked lines lengthwise along the front on the highest part of the fixture to provide a location mark that the fixtured parts must remain within, as well as a small circle at the 0,0,0 corner.

The width of each of those three shelves is 3.5". Well, I have a 3" face mill I want to use to rough them out, then come back in with a square end mill and hit the corners just to get them as close to square as I can, since the face mill inserts have a 0.030" radius on the corner.

I am having a hell of a time doing this. I think what I want is a pocket facing toolpath. But there is no single chain that represents the shelf I want to cut. I tried adding lines across the 1/2" slot to "bridge the gap" and let me select the whole base as the chain, then I planned to select the top of the rectangular posts at either edge as the 2nd and 3rd chain, thinking it would let the 3" face mill hog out the whole shelf. It isn't working. I can get it to pocket the whole thing, but then it doesn't push the tool over the open edges... I can't get it to work as an open pocket because two sides are open, not one, so I can't select a single chain that represents the pocket except for the open part. And I can't get pocket facing to work because when I go to select the geometry of the top of the rectangles at either side, the chamfer and v-groove marker line cut in the top makes the top of those rectangles not continuous chains.

I started to just draw the toolpath I wanted, but that makes it a PITA to come back with the square shoulder end mill to clean up the corners.

What approach would you use to machine out the shelves?

I can face it, slot it, drill the holes and chamfer it no problem... but when I get to using my face mill on those wide shelves, I just can't get what I want.

I've attached an IGES file in case anyone would like to see the model, it can be a bit tough to see what I'm talking about from the picture.

Thanks!

[tstom]

Mike,
Don't get locked into thinking that the only geomtry you can machine from has to sit right on the part Draw some rectangles that extend past the edges far enough to let the 3" cutter go where you want it to
Personally I would just face/pocket it with a smaller cutter ..say a 1" endmill that way you don't have to run so far off the part to clear the cutter edge and you eliminate a tool change I think you will find the cycle time will be about the same maybe even shorter you will still need geometry that extends past the edge of the part

If this doesn't help post again and I'll put a toolpath on your part

I just looked at the pic again... I would draw a rectangle arou the whole part enough bigger to let what ever size cutter you want to use clear all edges ...if you want to use a 1" endmill make the rectangle 1.05" bigger per side then put edge curves on the ribs and pick them as islands choose the area between the ribs as you pocket depth crank up the feed and stand back
the only thing you will have left to do is finish the slots

I'm anxious to look at Jay's version of your other part when I get to the shop tomorrow....I always learn something when I look at his work

[cadcam]

Mike tell us how big is the stock you are stating from. I always draw my stock around my part unless it to size. and we know how often that happens. then you do some what what Tstom was saying except I will not offset the geo I will use as it and you can pocket and live it standing. If it is to size contour will eat that right up for you with the tools you want to use.
Mike did you review my part. you will notice i used the new 2d HST to get the out side of the part.

If you are getting your files from SW your life should be much easer as you preatty much start off with every thing you need.

Have you become familer with the WCS system yet?

Did you know that when you bring in a SW file that the top from SW sits as front in MC?

Just a few thoughts.

[tstom]

See....I told you we'd learn something
Jay
Looking at your version of the other part I see you didn't draw any edge curves so I'm thinking I've been doing extra work all along Do you just use the solid edges that appear when you move the mouse over them? I didn't know you could do that

I haven't take the time to learn the 2d HST's yet ...looks like I need to


edit
Now I see .....just use the solids button for geometry selection .....lesson learned....Thanks again Jay

Tom

[SRT Mike]

Thanks for the replies,

cadcam, yes I took a look at your part, and based on your method I made some changes to how I had done it. I learned something from your taking the time to do the part in MCAM, and thank you!


As for this part, well I am actually not machining the outside portion... it is a 12" x 5.75" plate that is 0.750" thick. I got them as blanks, cut to (precise) size so on this one I don't need to do the outside. I am facing it 0.050", then cutting out the shelves, then cutting the slots, then spotting,drilling,tapping the holes, then running the chamfer around the outside.

Since I'm already going to have the face mill running for the facing op, I wouldn't be using more time to use it to cut the shelves, and I think it would produce a better finish on the floors of those shelves than a 1" EM... then I can just clean up the corners with another EM (maybe the 3/8" EM I am using to do the slots).

So from my perspective, I want the mill to come in on the long side, make a u-shaped path so it completely goes across the part and exits the stock, then makes a u-turn and turns around and comes back through. Then I can set it to leave 0.020 or so on the XY and clean that up with a finsihing pass with a 3/8" EM.

From the videos at streaming teacher, this would be a "pocket facing" toolpath. Does that sound correct?



and tstom, I have to admit I am feeling slightly stupid after reading your post, because the idea of just putting geometry over the existing lines and using that as the toolpath hadn't really occurred to me... duh! seems like that would work.

I'll give that a shot and see if it doesn't do what I want.