surface contour filtering

[ngkim]

in surface contour,when i select filtering,after posting,sometimes i get G18 or G19 in program,is it possible?afterall surface contour is z-level incremental cutting,will it gouge my work?

[mold100]

Have you verified your cut,I find best not to doubt the post,so if you verify your cuts and they look o.k. then you i believe that you should be good to go.Unless you have something wrong with your post.I could be wrong about this,considering I have never done filtering.

[cadcam]

What is the machine?

The post can be one factor but the Machine is the other.

[SpazMachine]

I have seen this before. If you have the transition set to follow surfaces and then filtered, sometimes on it's way down to the next cut it will make an arc. Check to see if the sideways arcs are in the same place as the Z- move and you should be okay. Otherwise I might be a little concerned.

 

Cody

[beav700]

I scraped two jobs using the filters in MC. Last time I buried 3/4 ball two inches deep into aluminum mold on our Hurco machine. Since then I told myself I will never use filters. It works for the most part, but one out of 30-40 jobs, the arc on Y-Z plane flips in the other direction and crashes in. Very hard to catch. This is where the G18 and G19 comes in. On the machines like Hurco the direction of the arc is opposite from most other machines and the G18 or G19 is needed in front of the line.

[cadcam]

So beav700, you want to use filter just do not turn on out put arc moves.

That is the colpret (sp?).

 

On some of the Fadals or in most of them I do not use this ,for some of the same thoughts.

Problems.

 

[ 01-30-2002, 09:37 PM: Message edited by: cadcam ]

[Guest CNC Apps Guy 1]

Verify verifies the NCI NOT G-Code. Very important. You could have a problem in your post but Verify shows everyhting is OK.

[Alan S]

I use the filter all the time on surface contour, but I leave the check box for 'create arcs' switched off, and that seems to be ok. The odd occasion when I've used it in the beginning, the Roeders machine we run on errors out anyway. It was only then I tried the filter without arcs.

[Travis_Buchanan]

I have also ran into problems when I project straight lines on to surfaces created from arcs. When I post code it will frequently changes planes which will screw up tool radius comp. My solution has been to move the line endpoints .0001" in opposite directions before projecting. This forces, depending upon you set tollerances, mastercam to stay in the g17 plane. I wish there was a selection in mastercam to force only g17 output, even if it an arc in the yz or xz plane, break it up into short linear moves dependant upon your max depth variation setting. Sorry I can't spell. How about putting a spell checker in this forum?

[Alan S]

Buzz

When you go /create curves/ project/ options,

you can then change the value in there to be alot tighter. This might help.

Spelling ? thats what I like about this forum, people just call it like it is.

Color or Colour - you decide.

[mold100]

Since Ive never had any expierience at this,what is the purpose of filtering,and when do you do it.(where to set it)?Thanks for any input to help me out.

[metalcut]

I also have same problem with heidenhain controller but no problem with fanuc controler.

[Alan S]

Mold100

It really all depends on how large your programs are and if you require programs that use less memory, therefore you filter to a specified tolerance, whereby the control jumps across areas less than this amount and so shortening the length of program. If you have 'create arcs' the control will convert to arcs again working to the tolerance set, this is where some machines are finding problems because of the need then to work in a different plane. ie. zy or zx

You will find it if you go in toolpaths, Surface/ Finish/ Contour/ select surfaces/ done. Then go into Surface parameters there should be a check box for filter if you 'tick' it you then turn the swithch on (just press the filter with cursor)

The filter works for other stratergies as well.

 

[ 01-31-2002, 08:08 AM: Message edited by: Alan S ]

[Zero]

I'm pretty shure that Alan is right.If you use the filter without the greate arcs checked it shouldn't create any G18 or G19 z arcs but will still create G17 xy arcs.I use the filter on all my toolpaths and the controlers can't handle z arcs and will just halt at that move.With the create arcs not checked I've never had any problem.

[Zero]

the h was supposed to be ere

[P_Scott]

For All,

 

Filtering is designed to reduce the amount of g-code in any given program by fitting single entities (lines or arcs) in areas where they can replace many tiny line moves. It does this by using the tolerances the user sets in the Filter tab. For instance, Mastercam breaks a Helix entry, or Z-arc, into many tiny line moves using the Linearization tolerance and Max Depth Variance values in the operation. If the Filter is not set in the operation, you may have over 1000 tiny line moves for the Helix entry. The Filter is desgined to reduce that number by replacing as many of those tiny lines with an arc, if you have turned "Create Arcs" on. This produces a G17, G18, or G19 in the code, depending on where the arc ends up being in 3-D. The control at the machine is what may have problems interpreting the G17, 18 and 19 moves, especially if it is an older machine. Because the Filter allows you to "Create Arcs" it not only reduces the size of the file, but in many cases, smooths out the result of the toolpath, gaining a better finish on the surface. The only time you may not want to use the filter on large surface files is if the machine control cannot interpret the g-code correctly, crashing the tool into the part. I used a Hurco SLV-40 in my last employers company and it definitely could not handle those types of moves. We could not use the Filter at that time. Now they have new Haas machines and they should be using the Filter all the time because of the type of mold work they produce. Sorry for the lengthy post but it seemed there was some confusion about what the Filter actually does. There may be more information about this in another location on the Forum. If anyone knows more about this, it might be an excellent topic for a Tech Tip or something.

[bryan314]

Filters are wonderful things. Depending on the part, surfaces, tolerances, etc you can get some nice reductions in your NCI and G-Code. 5, 10 50 or more percent. We have one machine with limited memory and this has saved me many times from having to breaking up the program into many files.

 

The ‘create arcs’ is ALWAYS unchecked or some of our machines have brain farts. Luckily we’ve never had a costly oopsy with the ‘create arcs’. We usually leave that to the ‘surface rough pocket’ operations.

 

Bryan

[Trevor Bailey]

beav,

 

The problem you speak of is Hurco specific. Do a search for the above mentioned text and you will find some useful info.

[gmenzies]

you might want to check out meta-cut filter.

we had some problems using mastercam filter back in version 7. so we bought this package.

 

the file reduction is usally between 80 to 90 percent of the posted g-code. a good investment

if you use machines like fadal or hass . it improved the overal performance of your machine.

 

[mikee]

The problem is the post. Change the line swg18 : 0

to swg18 : 1

That will fix the problem. Hurco is backwards

 

mikee

[Tony]

With filter off and my linerazation to .0001

The programs are 3 times larger and the part finish still has facet's.

Arc's are the way to go with Mold's.

I cut a demo to show the Hurco VP.

(Who told me Hurco likes all the information it can get more points along the spline the more accurate,Don't worry about G18/19 Don't use it)

So I showed him that the arc filtered program was way smaller and Didnt look like a stop sign either

I just did what mikee said above in my post.I search my program for any g18/19's output

and I check all my program's at the controller too be safe(visually)... Knock on wood

 

[ 02-06-2002, 02:15 PM: Message edited by: Tony ]

[beav700]

I tried changing swg18 to 1 and still had problems. The swg18 will fix the arcs on the x-z plane but not on y-z plane.

[Charles Davis]

I've found on some machines you want to use I'J'K arc centers (instead of R's) and set breakarcs =1 in your post, to break arcs at the quadrant points.

 

Set a higher Cut Tolerance than Filter Tolerance will often REDUCE the amount of code after filtering. The better the data the filter gets, the better job it can do (ex: cut tolerance =.0002, filter tolerance =.0005),

 

V9 does some nice things with "one way" filtering that v8 did not do, so I think you'll find the finish quality improves with V9 (just another reason to update).

[Travis_Buchanan]

I think I know why this guy is having trouble and

I thought about this today at work and I tend to dissagree with the statement that "you can post only g17 code by using filter options". I have created 2 almost identical parts to prove my point and posted code. I will upload these 2 files & the posted code to the ftp site when I get through explaining here.

 

Trash.mc8 is an octogon projected onto a sipmle raidial surface. Trash.NC is the actual posted code. I tried every filter option I could think of and I still get g18 output.

 

Trash3.mc8 is an octogon with the front & back lines changed to arcs with a .0001" deveation from a straight line. I then project this onto the same simple raidial surface, leave the filter off, and can post g17 only code. See Trash3.NC.

 

This was all done using Mill 8.0 Level 3, and my customized post. Does anyone know how to force only g17 output, without having to modify the octogon?

 

The mc8 files are in the (mc8 files) folder and the posted code is in the (all NC programs) folder.

 

One more thing. I know that the filters are designed to reduce program size by making longer straight lines or by "arc fitting". So if you filter code that already has arcs in it I dont think it will take them out.

--

Buzz Lightyear

 

[ 02-01-2002, 04:38 AM: Message edited by: Buzz Lightyear ]

[Travis_Buchanan]

Did anyone take a look at this? Do you see what I'm trying to say. I am not very good at explaining things, or understanding someone else explain them either. I am a "show me" kind of person.