Post Problem

[Müřlıń®]

I am having a problem with my post for my ancient control on my Cincinatti vertical mill.

 

It used to be a tape machine and I upgraded to a 31/2" floppy. The floppy drive only holds 250k when formatted in the Cincinatti format. I dont know what kind of OS this old machine has, FAT 12 or something maybe. DOS cant read it.

 

Since I only have a 250k buffer and no DNC on this control, you can see my delima. I must turn on Cir Int in the post and use the Section DLL Chook (which is bugged out BTW since ver 9)in order to keep disk usage to a minimum. Using circular interpolation decreased the code output 10 fold. Also on this old control, I am plagued with Disk Acess errors. So the less disks I have to use the better.

 

OK my problem.........my machining stratiges include alot of the Scallop toolpaths. Scallop is bugged since Ver 9 with Cir int turned on.

I have been advised to turn it off and run point to point. This is unexceptable for reasons I have stated.

 

I have altered a Dynapath post so I didnt have to start from scratch.

It has worked great from Ver 6 through 8.

When I upgraded to ver 9, thats where the trouble started. The post would throw in random plane changes(G17, G18, G19)where they didnt need to go. Since I didnt have a Verify that used the the NC file, Mastercam's verify only used the NCI file. Which showed no errors.

 

These errors of corse, caused me alot of headace's to say the least.

 

I had to make a VB script to edit out the "bad" code. So I must manually run my script after each posting.

 

Since I also have another machine with a dynapath control, I also use the same dynapath post for this control.

 

There is also a problem with this post(which I use unchanged right off the install CD).

This post inserts an E00(null tooling offset)sometimes on transformed toolpaths.

Another FATAL error, especially when you are away from the control:(

My script looks for this error and fixes it as well.

 

Can someone show me how to make a macro that will help me automate this process, or does anyone have a post that fixes these errors?

Or I guess some Rockafeller could give me 50K to upgrade to a state of the art control...........LOL J/K.

 

 

The controls in question are:

Dynapath Delta 20

Acramatic MC "big blue"

 

 

Thanks

 

Murlin

[Fig sign]

Murlin !

 

Welcome to the Forum !

quote:

---

It used to be a tape machine and I upgraded to a 31/2" floppy. The floppy drive only holds 250k when formatted in the Cincinatti format. I dont know what kind of OS this old machine has, FAT 12 or something maybe. DOS cant read it.

 

---

The ancient hardware and OS emulations is my sort of hobby.

I don`t want to argue with you but under dos you can read mostly all knows to me formats

including those of Macintosh and Amiga and write on all of them excuding Amiga floppy(amiga floppy drive oriented the floppy disk in special way that the regular drive can not do } "with a little help of a friend "!

And if you will find what the disk format it is I can give you a detailed solution .(Cincinatty guys must know what it is)

 

you say :

quote:

---

Since I only have a 250k buffer and no DNC on this control, you can see my delima. I must turn on Cir Int in the post and use the Section DLL Chook (which is bugged out BTW since ver 9)in order to keep disk usage to a minimum.

---

Methinks that what you call Cir int is a filtering and I find it far more better and stable in ver 9 than ever and have no alarms starting from ver9 !

You say "Scallop is bugged since Ver 9 with Cir int turned on."

Can you PLZ explain yourself?

 

And what bugs are in Section.dll C-hook ?

May be your post need some modification ?

Have you updated your posts with a C-hook UpdatePST9.dll ?

And I think that many times more effective combination to use surface contour + shallow .

Shallow toolpath tends to be more effective with arcs filleting and has more control .

 

Have you tried it ?

quote:

---

When I upgraded to ver 9, thats where the trouble started. The post would throw in random plane changes(G17, G18, G19)where they didnt need to go.

---

That`s because in filter options you choose to create arcs in XY ,XZ and ZY planes !

What else do you expect ,most machines demand to know in what plane your circular interpolation will be specified !

Turn of create arcs in planes XZ and Yz AND I BET YOU WILL NEVER SEE IT AGAIN !

quote:

---

Or I guess some Rockafeller could give me 50K to upgrade to a state of the art control...........LOL J/K

---

Your dealer can help you with a post !

And don`t be in a panic mood .

It looks like you Know programming .

Look at this as a sorta debugging process and don`t jump at once to conclusion that it is a Mastercam bug !

First of all check the possibility of not knowing something new or some little mistake somewhere.

RTFM of MC9 knew features and I wish you good luck.

And try what I told you it will be of no harm

 

Iskander the Entrance sentinel !

 

[ 07-07-2003, 05:25 AM: Message edited by: plasttav ]

[Müřlıń®]

Thanks for your reply. Since I'm HTML retarded I will do my best to re define my post.

 

Cincinatti will not talk about this control.

They want you to buy their new control.

There is no more support for this control from them.

 

I have had extensive communication with my Mastercam reseller about my problems and they cannot fix it. They even admit that Scallop is bugged with Circular interpolation turned on. They advise me to turn it off...DUH!!

 

It all boils down to the way Ver 9 posting has changed. They modified the post I have right now three times for me.

 

Ok.....My control uses the floppy drive for the memory buffer. A formatted floppy will yeild 250k. That is it 250k.

 

I do all my offline programming in Mastercam.

 

Yes, I could turn the filter switch off and not output arcs in the xz, yz planes and the random insertion of G18, G19 would go away on the Scallop toolpath.

 

However, the toolpath will have 10 times more code. In other words instead of a pirticular program only needing one disk, it will need 10.

My old control will stop with disk read errors alot. So the less disks I can run thru it, the less times I have to edit the current program and restart it. When I get a disk error I throw that disk away, delete the part of the program that has already run, and copy it to a new disk.

It is a very time consuming process that wastes alot of my day.

 

I use all the algorythms that Mastercam supplys to machine my dies. I build forging dies.

I could machine my dies without the use of the Scallop toolpath, but it would require considerable hand polish since my old machine is only capable of 20 IPM at best, most of my machining on this control is done at 10 IPM. So I have to be creative in my machining stratagies in order to machine my dies as fast and as good as possible.

 

Scallop will let me machine around a constantly changing x-y-z geometry and not leave any toolmarks. If I used contour and shallow in these areas, I would have to hand polish out the toolmarks because of the large stepover I have to use in order to make time. Trust me, I have been doing this for 15 years:)

 

If there was more money in this trade(forging), I would be able to afford to buy a new machine tool and I wouldnt be having these problems.

 

So the work around for my particular problem

was to make a VB script to correct this code problem. After I post and Section, I must manually run my script on all my post files. I was trying to figure out a way to have my script run every time I run my post.

This way I could never make a mistake.

 

Since I only have a 250k buffer, I must use the Section DLL Chook to split up my programs.

Perhaps Section DLL isnt really bugged. It might be ALL in the Scallop algorythm.

Since the DLL works off the NCI file.

All I know is that I must be extremely carful when I verify Sectioned programs.

STL compair will show NO gouges.

The Visual verify will show no gouges when it renders the end machined solid because the errors are in a rapid move.

 

The only way I have found to find these errors is to observe a manual backplot. Sometimes,

there is so many backplot lines on top of the other you cant see the gouge.

 

So the only 100% way to verify is to build the verify solid off the NC file. The only way to do this is to upgrade to the next Ver of Mastercam or buy an aftermarket verify program.

 

The first one scares the hell out of me, and the second alternitive is costly.

 

If anyone with any knowledge of CNC programming, has the knowledge of how to make Windows macros could help me out, I would be eternially grateful.........

 

Murlin

 

PS sorry for the long-winded post:)

[Müřlıń®]

Sorry a clarification........

Cincinatti is the machine tool manufacturer.

The control passed to Vickers, then to Siemens.....

 

Murlin

[Fig sign]

Murlin !

Talking about diskets can you tell what you can read on label are they double sided or not and how many slots you have two as on regular disket or one ?

I was very busy but had 10 minutes to look on some of my old stuff but i miss data to tell you what to do .

Sometimes if you disket is a modern one but formated less then 700k your pc floppy drive will regard it as double-sided and will not recognise it `s geometry.

Sometimes it is enough to cover with something like a masking tape the slot without a moving cover (the one that was not on old types of diskets) and it will read it OK !

 

About filtering :

There are other programs that can do filtering of your code outside Mastercam that are much stronger in this field Like Vericut and others.

Some PPL here are gurues in this field so they may help you with advice.

But anyway the nature of scallop toolpath such that it is hard for filtering.

The one thing I use is order cuts by minimum distance ,it helps for toolpath to look better !

And you can write e-mail to Siemence for support

about your drive ,they can have a special program for pc! Support web site

[Rick Damiani]

quote:

---

OK my problem.........my machining stratiges include alot of the Scallop toolpaths. Scallop is bugged since Ver 9 with Cir int turned on.

I have been advised to turn it off and run point to point. This is unexceptable for reasons I have stated.

---

The scallop toolpath dosn't respond well to filtering, and it sounds like your control dosn't respond well to the results of MasterCAM's filter. Having a small buffer complicates the issue, as the (unfiltered) scallop path has a talent for generating enormous amounts of G-code.

 

What I would suggust is this:

 

1) Change your machining stratige to use the contour and shallow toolpaths, and do one of the following:

- use the 'Shallow' button to add cuts to the shallow areas

or

- use the 'Shallow' button to remove cuts from areas you will pick up with a seperate shallow toolpath.

This can give you results that are nearly as good as the scallop toolpath in a way that will limit all the cutting motion to motion in the XY plane, which sounds like it would work for you. This is also what I usually reccomend in situaitons like yours where buffer space is limited.

 

2) Use the scallop path, but turn off the options to create arcs in the XZ and YZ planes, leaving the option to create arcs in the XY plane turned on. This will *also* eliminate the plane changes that are giving you so much grief, while retaning the XY arcs option and the G01 block reductions that filter is good for. You may not see a factor of 10 reduction in code size, but you should still get a signifigant reduciton.

[Fig sign]

+1 for Rick !

 

And you can use Tpcfg.dll to activate new options for surface contour toolpath(flat and shallow ) .

But anyway I doubt that you will get good surface scallop ever :

an old machine with a little buffer memory using floppy as a memory will tend to machine standing still waiting for a next block to come that will be easily seen afterwards on the part`s surface !

[Müřlıń®]

Riki......I use contour and shallows for finishing the impressions in my dies. In fact, I use ALL the toolpaths.

 

I see why you guys are not seeing my need for the Scallop. I am not machining small parts.

I am machining HUGE dies. Some weighing as much as 4000 lbs.

Also to complicate matters, the parting line on these dies is VERY irregular.

Compound curves at every turn.

 

An example of one of my dies would be drill heads for the Rockbit industry. For drilling oil wells and mining. There is not one strait or flat edge on the parting-line of these dies.

 

If anyone has a Bulldog trailer hitch on their horse trailer or utility trailer, I designed and currently manufacture the tooling for these forged parts.

 

 

Picture a block of Finkle Die Steel(with a hardness of about 42-45 RC) 36"x24"x14".

We only have 10 IPM.

We also only have 250k buffer.

I know....I know......I'm probably the only one stupid enough to use this machine tool for this app, but this is my life:)

 

These forging dies are kind of like molds but they are all in one piece. When it comes time to re-surface the worn out forging die, you have to lower the face of the die, where all the heat checks and worn places are removed.

 

Contour and Shallow in these areas would result in about a 300% incease in machining time alone. Not to mention the time required to hand grind the toolmarks out of certain areas.

 

Using Scallop with .100 stepover, along with the Highfeed option, is the only way I can machine the large, irrigular surface, and leave no tool marks in the corners around the parameter of the impressions that lay in the die block, and do it in a timly fasion given the my horrible working parameters.

 

So on a forging die, since there is so much area, you must use diffrent stratiges, on diffrent areas of the die, in order to make the best time on any given job.

 

I hope you all can see my need for Scallop now:)

 

Murlin

[Rick Damiani]

quote:

---

I hope you all can see my need for Scallop now:)

---

I can't see your geometry, but I'm willing to take your word for it that you need to use scallop. In that case, I'd suggust using filter and turning off 'create arcs in XZ' and 'create arcs in YZ' while leaving 'create arcs in XY' on. That should keep any G18 or G19 arcs from showing up in your code.

[Müřlıń®]

My appologies guys. Working alone all these years has not developed my communication skills the way I would have liked:)

 

It occures to me that I have given you all WAY too much information:) The point of my post keeps getting lost in the wash....hehe

 

I have re-evaluated the approach to my Querry and will repost in a more direct manner.........(LOL)

 

Thanks to everyone who replied..........

 

Murlin