V9 SP1A trouble

[lynnz]

I just uploaded a zip file to the ftp site called hub problem.zip

It contains 2 files--1 is a v9 SP1A file that has trouble with a pocket rough toolpath. The ribs on the parts are being milled off partially. The tool is getting into the part. I just ran the new patch this morning.

 

I also ran this same part in V8.11 It roughs the part without any trouble at all.

 

If anyone has both V9 and V8.1, could you see why the pocket rough isn't working correct now??

 

We just made a variation of this part about a month ago without any trouble at all.

I will probably dump V9 in the morning and reload it from scratch without the latest patch, but thought maybe someone can see if I'm overlooking something.

Running verify shows the problem.

 

Thanks

Lynn Zehr

[lynnz]

I loaded the file in the V9 folder on the ftp site.

 

Lynn

[Zero]

I have not looked at the file yet, but try some different cutting methods (Parallel Spiral,Constant Overlap Spiral, etc..). I have had the same thing happen using the zig-zag method in V9 and changing to Spiral type cutting methods fixed it. And I also was able to generate a correct pocket from the same part using Zig-Zag in V8.1.1.

[cam-eleon]

I had a look at it in v9. If you change the roughing angle to something like 45 deg all seems OK. I think this file needs to be sent to your dealer and or CNC for further testing

[lynnz]

cam-eelon,

For now I will run in V8 as it is proven to run as programmed. If I have to start changing angles and such to avoid cutter violating the part, that tells me there is a problem with the program.

 

Anyway I sent this to my dealer last nite at the same time I posted here. I think before the SP1 patch, V9 would have cut this fine. I should have been more cautious when installing a new patch.

 

I will let all know what CNC/dealer has to say.

 

Thanks

Lynn

 

[ 08-08-2002, 09:55 AM: Message edited by: lynnz ]

[cadcam]

Lynnz I have looked at the V9 file and I see it looks fine in the MC varify but checked in my varify and see it gouge the part.

 

Now I changed the pocket to a true spiral and does not gouge the part and is a nicer cut.

 

I have not even looked at the V8 yet.

 

Ok after running both the V8 does not have the same trouble and I am not seeing a diffrence in the paramaters pages.

 

I would send the v9 file to QC.

I have use surface pocket ruogh in v9 latly alot and had great luck and also in the last 6 months on other projects.

 

JM2C

 

[ 08-08-2002, 10:42 AM: Message edited by: cadcam ]

[P_Scott]

lynnz,

 

I checked your part and I changed the Feed Plane from an Incremental to Absolute value. That fixed the toolpath. Your Total Tolerance was a little large as well. A larger value gives you less accuracy with your surfaces to machine. Changing the toolpath method can reduce the amount of material that is left on the walls so the finish toolpath can perform better. I would also suggest looking into some of the other toolpaths such as a surface Contour or even the new Project-3D Blend toolpath for V9. HTH

[cadcam]

Peter I saw the feed plain issue but you are saying you could see the problem in the MC varify?

 

Just wondering.

 

Peter all of what you stated did fix the trouble in V9, but he does have it the same in the v8 and it worked.Got me.

 

Ok it was the tollorence diffrence between V8 & V9.

 

this is what killed it even knoe they are the same in V8 & V9 being the .010 the diffrence is how v8 & v9 see them now.

 

thanks peter.

 

[ 08-08-2002, 11:38 AM: Message edited by: cadcam ]

[Greg McKay]

lynnz,

 

I get some illeagel arc moves when backplotting file. We have a new appmch on the web. I have also forwarded it to Bob G. I have not had a chance to try the new app. app didn't solve problem. I will talk to programmer

 

[ 08-08-2002, 01:10 PM: Message edited by: Greg McKay ]

[lynnz]

Greg

I got the new file from Bob. I don't know whether I'll get a chance to check it today or not. Pretty hectic afternoon.

 

I tried Peters suggestion and changed tolerance to .002 from .011 in V9 and the problem went away.

I still think it shouldn't do it if one wanted to increase tolerance. Or maybe there should be a max tolerance that we could input.

 

I'll see what CNC has to say.

 

Thanks

Lynn

[P_Scott]

Jay (cadcam) and others,

 

quote:

---

but you are saying you could see the problem in the MC varify?

---

I did see that in verify it seemed to wipe out the tabs and just finish the general cylinder for the first couple of depths. After changing the Feed depth to Abs., the toolpath was fine. I don't know how much the tolerance affected it but it might have had a combination affect with the Feed plane setting. Granted .011" isn't a whole lot of room but it's a lot larger than .001". It's like the difference between peeling a potato with a paring knife rather than a peeler. A peeler is much more accurate but slower, and a paring knife is faster but removes more potato with the skin. I have also not had a chance to use the new Apps patch and try it out with this part. HTH

[Tony]

I have just finished converting an entire job back to MC 8.11.

There were places that MC9 would not remove stock.

when I tried it in 8 with the same parameters

It removed the stock on the first try