Bugs with verify mod

[David Colin]

I'm using V9.1 (not SP1 yet) and i'm experiencing some problems.

 

More embarrassing I'm experiencing bugs in verify mod that weren't present in V9SP1:

 

- sometimes as i zoom, stock disappears and as i go back to Mcam main view my part lost its arcs entities (and others)!

 

- I've got now a graphic problem in verify mod: as i rotate stock model shade doesn't work very fine. It's green or black.

 

- Still have some bugs with tools compensation both in backplot and verify mod (however post output is correct)

 

- More important: verification sometimes DOESN'T work. Toolpaths or special tools geometry (i don't know exactly the cause) are not correctly displayed. Areas which should be machined (and they are in V9.0SP1) are not displayed in V9.1

 

Do these bugs are fixed with 9.1 SP1 ? (still don't own it with french language)

 

Anyway, i'm joining files to show some of these problems (compensation / verification mod).

 

Here is the URL of .MC9 files to test (and correct) verify function in mill V9.1. You will have to associate tool-7 geometry file in tool-7 definition table. (I draw it on a separate level but it seems there is an other bug with Mastercam mill...)

 

Go here and download both main and tool files.

http://perso.wanadoo.fr/anorec/

With V9.0SP1 you probably will have to regenerate OPs (red crosses).

 

- You should see differences between V9.1 and V9.0SP1 after tool-7 verification (V9.0SP1 seems correct). With V9.1 chanfer machined with tool-7 isn't displayed...

- Tool-8 verification (and backplot) doesn't work with both V9.0SP1 and V9.1 however post output is correct...

 

Yours sincerely.

[Fig sign]

Salute ,David !

 

What is your grafic card and OS you are running ?

I use now Mastercam ver9.1 sp1 with Win2000pro and Geforce 4 mx440-SE no problems with verify.

quote:

---

- Still have some bugs with tools compensation both in backplot and verify mod (however post output is correct)

---

This can be related to Backplot->display->simulate toolpath compensation

and verify =>config->cutter compensation in control .

quote:

---

- More important: verification sometimes DOESN'T work. Toolpaths or special tools geometry (i don't know exactly the cause) are not correctly displayed. Areas which should be machined (and they are in V9.0SP1) are not displayed in V9.1

---

If you installed v9.1 from stratch make sure that your path points to the place were your tool libraries and drawings for nonstandart specific tools exists .

What can happend is that verify does not find data and geometry for your nonstandart tools !

In this case you can try verify ->config->profile->auto .

Make sure that your tool libraries and tools drawings are in your mcam9/mill/tools directory !

 

Iskander teh considerating !

 

[ 07-17-2003, 05:03 AM: Message edited by: plasttav ]

[David Colin]

I'm running Win2000pro SP3+Geforce4 TI4800.

 

Of course path/compensation control setting are correct and backplot (not verify) is correct too (with tools geometries) except with tool-8 in my example. In that case (tool-8), if i m turning off compensation control, toolpath in backplot and post output are correct (however not real tool move which is controlled differently by machines)!

[David Colin]

For information, I just installed V9.1SP1 and same problems are still there...

 

[ 07-17-2003, 12:29 PM: Message edited by: David Colin ]

[Fig sign]

Dave , only today I had time to look on your file !

In GORGE - 3 tool 8 lead in /lead out put on entry exit line perpendicular 0 and all will be OK.

Backup almost never make mistake .

Trust it !

This is a little mistake of yours, not bug .

You choose point for in out and simply MC can not do what you want.

Generally while you are in compensation type -control always try to make lead in/out with line only or line arc avoid arc only.

Not every machine can do it and it can scrap your part !

Iskander teh smiling !

 

[ 07-21-2003, 12:39 AM: Message edited by: plasttav ]

[Fig sign]

David !

 

Are you satisfied with my answer ?

 

?! Reply ?!

 

Iskander teh waiting ....

[David Colin]

>Are you satisfied with my answer ?

 

Not really... Of course if i enter without an arc it works. But i need this entry with 180deg-arc in this machining case to progressively take chip.

 

I'm not ok with you:

 

Mcam has all informations to create this toolpath and it's doing fine. I said post output was correct.

 

In my example, every machine with compensation control capabilities can theorically run post-output made by Mcam (but sometimes cnc machine tool bug too...). Parts of the example have been machined last week and the gorge doesn't look like verify/backplot seen in MCam. That's all.

 

by te way,i spent about 10hours today in front of Mcam and i'm pretty sure that verify (backplot is ok) doesn't work at all with special tools geometry.

 

So be careful if you are drawing your tools!

 

I also received a mail from CNC software and they wrote the bug into their log book. Wait and see.

 

[ 07-21-2003, 12:36 PM: Message edited by: David Colin ]

[Fig sign]

David .

I am writing from home can not check your file once more ,I will check tomorow .

quote:

---

In my example, every machine with compensation control capabilities can theorically run post-output made by Mcam (but sometimes cnc machine tool bug too...)

---

Not every one and they are not bugged !

Some CNC machines have a limitation :

you can not enter to G42 or g43 with first movement -arc !

I know thats sounds a bit crazy but it is a sad fact !

One of my machines is a good example of this.

Yes , in fanuc6 from 25 years ago I entered from arc but not all machines can do it even now.

But even on FaNuC6 the real movement was a curve like ellipse .

I will check your file once more tomorrow.

Anyway I think than if you have space and you can have two movements line and arc put some line lenght mill radius +0.1 and arc radius and you can have a good result !

I say that I must check it tomorrow .

Now there exists more funny things .

I don`t want to argue with you just for your information :

I can give you examples when you will get undercut in backplot but the part will be OK like on my Deckel-Maho dmc63v with Sinumeric 810 !

But you will get this undercut in other machines.

You know that when you choose compensation by control and check in toolpath optimization MC will not gouge the toolpath.

Now if I will not check optimization and the gouge will be less then 12 blocks my machine`s built-in optimizator will not allow the gouge !

Now on the backpolt you will see the undercut but will not get it while milling!

 

[ 07-21-2003, 04:34 PM: Message edited by: plasttav ]

[Rekd™]

quote:

---

you can not enter to G42 or g43 with first movement -arc !

I know thats sounds a bit crazy but it is a sad fact !

---

The reason for this is that when using CRC on an arc, the start and end points of the arc, as well as the dia, are different than if there is no CRC. So you would end up with a gouge, or incomplete arc.

 

'Rekd teh "Gulp! My wife's sick...again!"

 

[ 07-21-2003, 05:15 PM: Message edited by: Rekd ]

[Fig sign]

David!

 

Turn off optimize and you will get what you want!

 

If you have questions I will explain later.

 

C U !

[David Colin]

>you can not enter to G42 or g43 with first >movement -arc !

 

I'm OK with that too! But in my example MCam is making the missing line move (entry towards start of the arc point). This is a standard move.

 

>You know that when you choose compensation by >control and check in toolpath optimization MC >will not gouge the toolpath.

 

In my example optimization doesn't change anything because arcs (entities chained and leads/in-out) are smaller than tool's arc. It's very important to have exact toolpath post output.

 

I must go to the office right now. See you soon.

[Fig sign]

quote:

---

In my example optimization doesn't change anything because arcs (entities chained and leads/in-out) are smaller than tool's arc. It's very important to have exact toolpath post output.

 

---

Yes it DOES change !

I don`t say without checking .

I did it on your file with success !

Turn it off and see yourself .

As I said before I will explain later.

 

C U !

[David Colin]

>Yes it DOES change !

>I don`t say without checking .

>I did it on your file with success !

>Turn it off and see yourself .

>As I said before I will explain later.

 

Really weird. Nothing changes here... perhaps you changed control compensation simulation off ?

[Fig sign]

Do you want more ?

If you change only arc sweep angle entry /exit from 180 to 90 degrees even with optimization you will be OK !

 

 

Ready to explain !

PS done on Mastercam v9.1 SP1 , backploting with compensation simulation on

 

Iskander s!Z Men sana yaratam ,Mastercam !

 

[ 07-22-2003, 07:54 AM: Message edited by: plasttav ]

[Fig sign]

I put a file with my changes to Jay`s FTP

have a look

ftp://mastercam:[email protected]/Ma...orum/MC9_files/

 

and take file ISKANDERGEOMETRY TOOL7.MC9

Sorry for a strange name

You can see by your own eyes that what I say is true !

 

PS Sorry ,Jay , I created by mistake empty directory New Folder and can not delete it cause I have no rights !

 

[ 07-22-2003, 08:17 AM: Message edited by: plasttav ]

[Fig sign]

David !

I had time now to check my file on MC ver9,ver9.1 and Ver9.1 sp1.

 

Backplot is OK on all of them !

 

 

Iskander teh relaxing ..../....

[David Colin]

Thanks to you. I checked your file. It works fine to me! But this is definately a bug ... Optimize checkbox has no effect (it s ok). The prob seems to be lead-in arc angle: If you type 155° it works, you type 156° and above it fails (lead-in/out is backploted but 360° contour is missing)... no reason.

 

Anyway, did you compare special tool-7 verify (chanfer) with both V9.0 and V9.1?

 

I found today some other weird things about verify but i'm keeping them for CNC software.

 

[ 07-22-2003, 12:03 PM: Message edited by: David Colin ]

[Fig sign]

Salutation , David

quote:

---

But this is definately a bug ... Optimize checkbox has no effect (it s ok). The prob seems to be lead-in arc angle: If you type 155° it works, you type 156° and above it fails (lead-in/out is backploted but 360° contour is missing)... no reason.

---

Yet it is not a bug ,in my humble opinion and it has sense !

Do you fully understande what is optimize?

Have a look here ,plz !

Optimization prevents gouging .

Let`s have a look on your toolpath .

Your geometry is center point and contour (full arc ).

You choose line in out 0 and arc radius 17.9 and sweep angle 180 degrees.

What happens is this : MC builds line from center point to enter arc 17.9 180 degrees and exit in the same manner.

You are in entering arc with compensation and in exit arc too.

When it calculates the real movement it finds that it cuts the entering arc while it is in contour and exit arc and prevents gouging.

For MC it is a gouge and for me it is too.

For MC every movement after compensation call checked for gouge no matter if it is entering movement ,real toolpath or exit movement !

Here comes two decisions :

You can turn of optimize and gouging is your responsibility now ,it will not be checked now and you will get what you want or you leave it as it is and reduce the value of arc entering exit movement with the same result .

You can argue if you like and say that this is exageration but I can give you examples when you really nead this way of gouge regarding .

It suits me and I don`t think it is bug !

Weird things happend sometimes from not proper understanding of some things .

I say once more :MASTERCAM HAS BUGS ,BUT TRY NOT TO SEE IN EVERY THING THATS YOU ARE NOT OK WITH IT A BUG!

quote:

---

Anyway, did you compare special tool-7 verify (chanfer) with both V9.0 and V9.1?

---

I will look tomorrow .

quote:

---

I found today some other weird things about verify but i'm keeping them for CNC software.

---

Come on ,don`t be so greedy .

Throw them here . May be we can help you without CNC Software !

 

Iskander teh CNC Software defender !

[David Colin]

Hello,

 

I exactly know why optimize checkbox is used for. First part I killed made me understand: avoid check it as you're machining finish contour with tool radius = arcs entities radius in contour: If real cutter radius used by operator is slightly inferior to arcs in contour then arcs of the part will become the same as tool radius. With optimization: if arcs (a pocket) in the geometry chained are inferior or equal to tool radius, MCam calculates points that cnc machine tools can manage to calculate tool compensation. It works fine.

Of course, With some couple contour geometry/tool if you don't check optimize MCam can't create a toolpath (or partially). That is normal. However in that case, there is no (or partially) post output. Not the same as in my example in which post output is complete and correct. I repeat: in the example if you check or not the 'optimize' checkbox there is no difference because there is no optimization to make (radius tool < lead-in/out arcs and contour arc). Optimize checkbox has nothing to do with gouge control in lead-in/out. There is another checkbox for that in lead-in/out form.

And in my example it also has no effect cause there is no gouge and mcam doesn't find gauge. It's OK. Prob is backplot only.

[Fig sign]

quote:

---

Optimize checkbox has nothing to do with gouge control in lead-in/out. There is another checkbox for that in lead-in/out form.

---

If you select optimize toolpath you wish to see on the backplot results of optimization ,if you turn it of ,backplot will not show it.

Backplot without displaying compensation will show you that the movements are OK , but on machines with optimisation and "bottle-neck" checking you will get or not complete toolpath or alarm message, it depends .

If you manage with a success to run this specific toolpath on your specific machine it only means that your machine doesn`t check for undercut the compensated toolpath the way other machines do!

For machine all the movements after G41 or G42 call have the same sense, from what the heck it can know, that your arc is the entering or exit move?

quote:

---

Thanks to you. I checked your file. It works fine to me!

---

That`s your words .The facts support my theory ,right ?

But you don`t want to listen . EVEN real facts have nothing to do with you .

And "you exactly know all "!

I learn new simple things every day but you exactly know this and that .

I am tired ,David !

I tried to help you but I failed .

I stop this fruitless discussion , I have other

things to do .

It doesn`t matter me much what you `ll say , call this a bug 1000 times, me it doesn`t matter !

Why I must argue ?

I do this stuff without the problems all the way from ver 7. and will do it in the future.

 

 

Iskander teh retired !

 

[ 07-23-2003, 06:29 AM: Message edited by: plasttav ]