Lazy Iskander dirty tricks Inc .

[Fig sign]

********BRYAN`S C-HOOKS *********

 

The C-hook will be menu.dll.

 

It`s my special favourite I use it all the time.

 

You can add menus ,put menu inside menu ,add second ,third pages and more.

You can find my everyday working menus if you`ll download

 

ftp://mastercam:[email protected]/Ma...hooks/lazy9.zip

 

 

This is 4 pages three levels menu of some useful stuff,that I added to mastercam menu

Every separate menu must has menu.dll and menu.txt put to the chooks directory in your Mastercam.

Creating the second menu you simply copy your menu.dll and menu.txt files to some other names like menu1.dll and menu1.txt

And for every menu you must edit it`s *.txt file.

You can do it in every text editor.

Notepad will be good .

 

Example from my menu.txt

quote:

---

[menu]

menu 1 {"Chooks:","secpa≥*", "&layout*", "&breakcir*", "C&a3pts", "&color", "&level", "se&tdirs*", "&setmain", "colrsur&f*"}

f*"}

---

"Chooks:" this name will appear over the menu

 

& will make the letter appear underscored for hot key-ing like &color you will see in the menu like _color

 

All & in the menu must be unique.

Commands you wright like &color and c-hooks like

"se&tdirs*", max ammount of fields is 10.

 

"secpa≥*", here I am pointing to the second menu

c hook that`s menu second page

 

Second page text

quote:

---

[secpage]

menu 1 {"second page:", "&Crpt2pts*", "c&a3pts", "&bryan*","bryan&2*", "m&ousemch*", "&delalld*", "d&etdiam*", "gr&id*", "&hardware*", "keeplev&s*" }

---

"&bryan*","bryan&2*", - here I am pointing to the third level of menu two pages of Bryan`s c-hooks

 

Put the menu.bmp file to the *commonicons directory , the rest to c-Hooks directory *chooks .

Now screen->configure->toolbar/keys define it in some free place at your toolbar and you`ll have nice additional menu .

Or assosiate it with a keyboard keys combination like F10 key

 

Have fun

 

Still to come : mill9.txt or hack your Mastercam .

Stay tuned !

 

 

ITHH

 

[ 10-23-2003, 05:47 PM: Message edited by: plasttav ]

[Fig sign]

Lazy Iskander Dirty tricks revival !

 

I am glad to present the next dirty trick :

Use of trim functions for clamps change.

Have a look at ftp://mastercam:[email protected]/Ma...iles/lazy10.rar

 

There are cases when it is the simplest way to implement the clamps change ,especially when you don`t have all the geometry ,but used some transformation function like rotate !

 

 

I will also appreciate any input ,may be someone has some ideas or questions , I AM AT YOUR SERVICE !

 

ITHH

 

[ 10-26-2003, 05:52 AM: Message edited by: plasttav ]

[Fig sign]

Lazy11 trick

 

Creating a model for milling electrode

 

Mastercam like many other programs has limitation :

you can not mill surface toolpathes with offset minus value bigger than corner radius .

It means that if you milling with an end mill sharp corner(radius )you can not mill with a negative surfce offset at all.

This trick gives tyou a possibility to make EXACT MODEL of your electrode and so you will not need NEGATIVE offset .

 

Have a look at ftp://mastercam:[email protected]/Ma...iles/LAZY11.ZIP

 

Lazy11 trick

 

How to build fast model for electrode minus 0.3 (spark 0.3 mm) milling fast

 

1. solid created

2.solid copied to level 20

3. solid shell inside direction wall thickness 0.3

4 original solid and shelled solid copied to the level40

5 .proceeded with boolian remove original minus shelled.

6 the result is a model for electrode milling

 

I will also appreciate any input ,may be someone has some ideas or questions , I AM AT YOUR SERVICE !

 

HF!

HTH !

 

ITHH

[Lars Christensen]

some of this stuff is above my level, but I am eating it up, keep it coming, keep it coming, you got my attention.

thank you

thank you

 

Lars

[Fig sign]

Lars !

Thanx a lot!

 

You are the toolmaker .

I know what it means .

 

Mostly all the tricks must be simple and fast to do otherwise it has no sence .

In what are you interested spec. ?

 

[ 10-26-2003, 11:08 AM: Message edited by: plasttav ]

[Fig sign]

********BRYAN`S C-HOOKS *********

 

 

The c- hook of the day is scanarcs.dll.

 

It is rather neat and nice little c-hook which can help you sort arcs

 

Choose custom color and proceed with a c-hook .

After selecting of arcs you`ll see nice options to sort arc equal too ,less,greater ,in range or outside of the range ,that you must input now.

the sorted entities will get the presetted custom color .

Good for analizing and sorting and that`s what masking misses !

 

HTH!

HF!

ITHH!

[bryan314]

Holy cr*p IskandeR. I'm gonna have to hire you as my PR guy. Now if you could only get people to start sending truck loads of money. Then I could stay home and write chooks all day.

 

Anyways. What exactly did you mean by 'multiline option' in the Create at Length chook posting?

 

Bryan

[Fig sign]

quote:

---

I'm gonna have to hire you as my PR guy.

---

I will advise with my lawyer and will send you my

conditions .

Regarding payment Lazy Iskander Dirty Tricks inc. accepts dollars , shekels and limericks (limericks are preferable option )

Also keep in mind that I can put your ad`s

here for a small price , very goog idea !

(Am I smart guy ?).

 

Seriously

quote:

---

What exactly did you mean by 'multiline option' in the Create at Length chook posting?

 

---

The ability to built multilines with arcs on the lines ends like in create ->line->multi

 

The Bryan`s advertisement _ a possible example.

quote:

---

FOR HIRE: CUSTOM CHOOKS

If you would like a customized version of one of my chooks or have the need for your own chook please contact me for details.

My web page

While I'm not limited to the areas above, please use them for a rough guide for what is possible.

 

In addition to the above chooks I've dealt with:

Plane and view manipulation and creation. Including named planes.

Reading and writing parameters in the operation manger

Drill point manipulation: sorting, deleting and auto adding drill points

Pattern recognition

Pattern creation based on variable input - think similar to the gear chook from MC.

Checking and manipulating job setup values

Importing and exporting entities

Exporting entity, tool, operation information and other available system variables

Integration with other systems

Last but not least post processor customization.

 

Bryan

 

--------------------

work:

www.steeplechasetool.com

bryan (_at_) steeplechasetool (_dot_) com

c-hooks:

www.ivanxxxx.com

bryan (_at_) ivanxxxx (_dot_) com

 

--------------------------------------------------------------------------------

---

OOPS advertisement is banned ?!?

 

[ 10-26-2003, 03:19 PM: Message edited by: plasttav ]

[Lars Christensen]

Hi Iskander,

 

I believe my biggest problem running mill, after have been let out of the edm cage is experience.

Just looking for basic's, like doing rough stepdown in taper, so you dont put unnecesry pressure on the endmill....(dont know if this was correct expressed, oh well ).

I guees you could call me "Lazy" I am trying to steal experience. It helps me alot, seeing how you guys are aprocing a job, I am working nights right now, and the onely guy who I trust with mill questions is gone when I come in, and he dont even know Mastercam.

I wish I could put my finger on what I need to know the most .

 

Lars

[crazy^millman]

Lars I will offer this and see if it helps you here. If you have a 3d part and you want to create what soem peopel refer to as stair step down a 3d part I have found with what we do that surface rough pocket works the best. Example part is a complex part that you are cutting out of a bar stock and you want to cut all the 3d surface and also cut the bar stock but do it in one toolpath and process.

 

The toolpath I use the most is surface/rough/pocket with a boundary. I will either use inside if wanting to create like a support rid outside of the part for support. If I want to machine it all off I will use the bounding box I have created as the control or the boundary of the bar stock then use center as control. I liek to use the parrelle control on the pocket toolpath. If I am worried about center cutting I will align all the start point to the outside but will create a bounding bow bigger than the part and it will plunge in space create a little more air time but if you are cutting at 200 ipm that goes real fast.

 

I use other toolpaths to rough but like this one the best for complex parts. I find that others ones rapid to much for me or require alot of semi roughing or create place just not cutter friendly more often than not. I hope that helps give you soe midea. Keep pluging away at it and dont be affraid to take some chances soem of the best lessons you will ever learn will be be trial and error I promise you that.

 

Crazy Millman

 

[ 10-27-2003, 12:34 AM: Message edited by: Millman^Crazy ]

[Fig sign]

Lars !

 

What version and level of Mastercam do you have ?

Do you have solids ?

You are welcome to ask concrete questions I `ll be happy to help ,if I can .

 

Millman !

quote:

---

I use other toolpaths to rough but like this one the best for complex parts. I find that others ones rapid to much for me or require alot of semi roughing or create place just not cutter friendly more often than not.

---

I can show you a couple of tricks if you don`t mind,sorry if it is an offence, to have easy life using surface ->rough->contour and parallel.

 

At contour you can use arc for entering -leaving the contour ,at parallel inside gaps settings you can use an option of tangential tool path extending (gives uou an option always enter outside the blank material)

 

Stay tuned and have a look in the near future at Lazy12 trick

 

ITHH

[Fig sign]

LIDT inc. is proud to announce the next dirty trick :

 

Lazy12 trick .

 

Using special features to enter always outside material in surface->rough-> contour and parallel

To get this use in contour enter-exit line-arc feature on the last page of toolpath parameters and

in parallel use inside gaps settings tangenal line lenth .

 

Have a look on

ftp://mastercam:[email protected]/Ma...iles/LAZY12.ZIP

 

 

HF!

HTH!

ITHH

[Lars Christensen]

Thanks guy's all these tricks are going right into my note book .

 

The company have for the last 4 years tryed to find a good mill guy without any luck, the boss got sick of some of the issues they had in the mill dep. like have to scrap 7 pieces to get one good, or have to reprogram a job that already have been on the floor, because one hand dont know what the other one is doing. So his solution was to get me out there what is ok, but it is 8 years since I was runing a mill and that was with handels. Because there havent been any with good knowlege the hard jobs are gone, so alot of the stuff is very basic, I have onely had 1 job the last 3 months that requred surface milling, but I am planing to change that.

 

I have Mcam 8.1.1 level 3

Haas Mini mill with 6000 rpm max.

[Chris Rizzo]

Thanks for all the tips and tricks, you're very generous with your time and knowledge...and there is ALOT of both here!!

 

On occasion I've missed a few "episodes" here, and had to chase them a bit on the FTP...what about possibly getting your own folder on the FTP for Iskander's "tricks/tips/demo/tutorial" files?

 

Thanks again!

[Chris Rizzo]

P.S. You're probably saying "just use the URL links". However I use Opera for browsing, and it does'nt support the direct log in to the ftp. I open the FTP in a seperate window, and click around a bit for the files.

[Fig sign]

quote:

---

You're probably saying "just use the URL links".

---

I will say use Mozilla and you will not have any problem at all.

And far more safe and better then Explorer and free.

I tried Opera once for Windows and Linux.

It had only one good point ,IMHO .

At the era of week computers it worked faster than

Netscape or Explorer .

Now this is not actual .

 

Iskander teh destroy your own pc

Debug

wcs:100 1 01 06 (never try to do it !!!)

 

[ 10-28-2003, 04:28 AM: Message edited by: plasttav ]

[Fig sign]

Thanx ,guys for your input!

 

Lars ,so you can not see my *.MC9 tricks ?

 

It has a sence to upgrade to ver 9 !

A lot of improvements.

And if you build your 3d parts a lot solids is a must .

It saves a lot of time !

Anyway try to get from your dealer a demo of ver9 and you will see it yourself.

 

I can convert some of my tricks to ver8. some not cause not all the features I use exist in ver 8.

And it will take a lot of time .

quote:

---

like have to scrap 7 pieces to get one good

---

That`s not because of Mastercam !

Instead I can say that for a couple of years I scrapped nothing that I can blame it !

BTW what problems do you have with mastercam milling in your place spec.?

[Lars Christensen]

Iskander,

Sorry, I forgot to write that I have Demo9 here at home, thats how I have seen your tricks.

 

I dont blame mastercam for the mistake that was made in the mill dep. infact I am very impressed with mill version compared to the wire.

But when people are sitting translating every drawing to zero because they dont know that there exist a T/C Plane buttom, and editing the post to get G55 in there.

The 1st day I sad down and asked questions like:

STL?

Batch?

Highfeed?

Filter?

Tool liberary?

Operation liberary?

and so on.

Answer= We dont know, we dont use it.

 

I am not pointing fingers, nobody had just taking the time to figure these things out, even think that you can put alot of the blame on managment.

 

Lars

[Fig sign]

Lars !

 

quote:

---

The 1st day I sad down and asked questions like:

STL?

Batch?

Highfeed?

Filter?

Tool liberary?

Operation liberary?

and so on.

Answer= We dont know, we dont use it.

 

---

First of all try to get some milling course .

Anyway I am self-taught Mastercam user ,went the hard way and I want to say :

read the books .,

read the help on every thing that you don`t know.

write a test programs on simple things simply to see ,how it is working

And you have this forum !

Let me say you want to learn about filtering -

Make a forum search search with word filtering and see how much you will get .

This sort of basic stuff is covered prelly good .

And you can ask questions.

When I have at work a spare munute , I lite a cigarette ,make a cup of coffe and start to wander through mastercam .

If I found something that I don`t know I look about it in help file and test it.

Every button ,every parameter and check box in main jobs like contour,pocket.drill,surface contour,parallel ,scallop,shallow ,pocket you must know and understand .

And you will feel Masrercam might and your ability to use it.

 

 

There is a saying my friend uses to say:

With a wish and a lot of trying

even a pig can learn flying

 

I wish you good luck on your same hard way road

and I hope you feel less desperate in quite near future .

 

PS Have a look on my next trick .you will have fun

 

ITHH

[Fig sign]

LIDT inc, is proud to announce

 

*******************Lazy13 trick********************

 

 

have a look at ftp://mastercam:[email protected]/Ma...iles/LAZY13.ZIP

 

Milling helix using different ways to do

it with and without filtering

 

 

The curve is bult with

creatr->next page->spiral/helix command

 

Have al look on result of filtering of 3d contour with offset

the code takes 3 times less space !

Some types of toolpathes will not reduce the toolpath size,

as you can see in example

To get the good toolpath infinite look ahead must be unchecked

 

Rotary A contour with offset type control has no sence and will not be executed even if it is choosed

 

HF!

HTH!

ITHH!

[Fig sign]

This is reply to the article

 

 

******************LAZY14 TRICK**********************

 

 

have a look at

ftp://mastercam:[email protected]/Ma...iles/LAZY14.ZIP

 

This is a planar toolpath but you can easily produce the true 3d toolpath .

 

! offset target geometry to needed amount

2 break contour in the middle

3 translate it to the step Xform->translate->copy

4.build entry -exit lines

5 contour 3d toolpath without compensation and lead in lead out

 

 

HF!

HTH!

ITHH!

 

[ 10-29-2003, 01:01 AM: Message edited by: plasttav ]

[Lars Christensen]

Iskander,

The search button on this forum have been my best friend these 3 months, this forum is amazing, feel like I owe a couple off rounds to everyone.

 

I more or less have got the different buttons and options in mastercam under control now, know I am just looking for the dirty tricks and the right jobs to use them

 

Just came home after 12 hours in the shop, and with alittle luck I can get 4 hours of sleep before my 2 year old sneaks by her mom to come and weak me up, so I am gonna look at the files after some sleep.

 

Thanks

Lars

[Lars Christensen]

Lazy 13.

 

Iskander, ok I took a look and if you have a second could you confirm these observations.

 

Filter: did not changes my output in length on or off. Because there aint any small line segments or small rads. ?

 

Infinite look ahead: the reason for the bad output is because it is a helix shape, right?

 

Rotary A: Just makes my output 10 kilomerters long, reminds me of a 4axis in wire.

 

And then some secondary questions.

I have the Clearance buttom checked as default on parameter page, just to make sure that the machine aint crashing, any reason you dont?

I see you are using Material for feeds and speeds, I am using tool for the reason that SFM and chiploads seems to me can changes depending on what kind of cut you are using with a specific endmill. Is this just how ever you desire or is there a good reason for that.

 

Thanks

Lars

 

"You said I could ask questions, you did not say that they had to be good once "

[Fig sign]

Lars .

I will start with a secondary question ,it is far easy to answer

This is a demonstration file ,not for work .

I didn`t licked it up.

And don`t pay attention to speeds ,feeds ,clearances and so - they have no sense !

 

This is not a set of operations run one after other ,this is the one operation run several

ways .

I did it in 10 minutes and checked it in principle ,not paing attentions for speeds ,feeds ,material.

BTW I never pay attention for a material , I have

my custom self- made

tool libraries for main materials like wood ,plastic .copper, graphite,alluminim, mold steel ,hardened steel etc.

Never use calculate from material and so B$.

BTW never got it to calculate even approx.

to the real numbers .

Libraries ,recomendations of manufacturer and experience that`s what I use .

quote:

---

Filter: did not changes my output in length on or off. Because there aint any small line segments or small rads. ?

 

---

That`s not true

I choosed hellix because it is one of the worst cases for filtering.

This is parametric spline which Mastercam will divide to line segments building the toolpath .

Now here is an important point :

If you compare the NCI file sizes of compensated toolpath (compensation type control (G41)) with and without filtering jobs 2 and 4 they are 96 K and 34k !

So even here filtering made a result 2.8 times !

in most cases of 2d splines and 3d filtering the result will be much better!

The question is why in other cases the filtering done nothing ?

I can explain this too

When using the g41-g42 compensate to control style the toolpath consists of line segments which is easy task for filter .

When you use compensate to control or wear Mastercam builds the OFFSETED TOOLPATH like you can build it in Xform ->ofset contour : with radiuses in all corners!

So for every n line segments n-1 arcs will be added . You can see it youself if you `ll save your backplotted toolpath to some different level and will analize from close entities or with screen->statistics command !

And this arcs are tangent to this 2 lines so filter can do nothing !

And in contour with rotate about Z axes filter will do nothing cause we have the same offseted toolpath that afterwards all Y movements are substituted for A movements .

The size of NCI file is the same and all the explanation from the upwards are aplyable here

too !

 

From all this long story comes one interesting

thing to remember :

in 2d 3d contour toolpathes compensated to the control will be filtered best !

 

quote:

---

Infinite look ahead: the reason for the bad output is because it is a helix shape, right?

---

the help definition :

infinite look ahead

In contour analysis, to search the entire boundary to find self-intersections based on the current offset distance and cutter compensation.

It means that this is most useful stuff it saves you from undercutting ,overcrossing of the toolpath and so , like will not allow you to mill one side of a slot and undercut (trash ) the other on all the contour length .

But in this case it regards hellix as overcrossing contour and will simply not allow to mill it right ,while checked .

The same task like infinite look ahead has optimize for compensate to control toolpath .

 

Ps I like your questions , a real pleasure .

Thank you

 

ITHH

 

[ 10-30-2003, 05:50 PM: Message edited by: plasttav ]

[Lars Christensen]

Iskander,

 

Ok, now I see what the filtering does in Lazy 13, it makes the NCI shorther and it changes the nc gode. Now in the real world:

In op2 the NCI is 3 times as long, this makes verify taking longer, but not the nc output longer, this will still make a good part, right.

 

Lars