too much code!!

[LFP]

I am milling a 3d contour with depth cuts of .015 with a taper wall angle of 65 degrees. How do I get less lines put out into my Cimco file? Below is what I am getting for output lines.

 

G1Z6.1211F33.

X6.4634Y.254F20.8

X6.5579Y.5143Z6.1546

G2X6.5623Y.5254I.1983J-.072

G1X6.6715Y.78Z6.1881

G2X6.6765Y.7909I.1938J-.0831

G1X6.7999Y1.039Z6.2207

G2X6.8055Y1.0495I.1889J-.0939

G1X6.9429Y1.2904Z6.2523

G2X6.9491Y1.3005I.1832J-.1045

G1X7.0998Y1.5333Z6.2829

G2X7.1066Y1.5432I.177J-.1146

G1X7.2703Y1.7672Z6.3123

G2X7.2776Y1.7766I.1703J-.1245

G1X7.4538Y1.9911Z6.3405

G2X7.4616Y2.0001I.163J-.1338

G1X7.6497Y2.2044Z6.3674

G2X7.658Y2.213I.1552J-.1428

G1X7.8574Y2.4065Z6.3928

G2X7.8661Y2.4145I.1469J-.1513

G1X8.0762Y2.5966Z6.4167

G2X8.0854Y2.6041I.1381J-.1593

G1X8.3054Y2.7742Z6.4391

G2X8.315Y2.7812I.129J-.1668

G1X8.5444Y2.9388Z6.4598

G2X8.5543Y2.9452I.1194J-.1739

G1X8.7923Y3.0897Z6.4788

G2X8.8025Y3.0955I.1094J-.1803

G1X9.0483Y3.2265Z6.496

G2X9.0589Y3.2318I.0992J-.1861

G1X9.3117Y3.3489Z6.5114

G2X9.3226Y3.3535I.0886J-.1914

G1X9.5816Y3.4563Z6.5249

G2X9.5927Y3.4604I.0778J-.196

G1X9.8572Y3.5485Z6.5365

G2X9.8685Y3.552I.0667J-.2

G1X10.1376Y3.6252Z6.5461

G2X10.149Y3.628I.0554J-.2035

G1X10.4218Y3.6861Z6.5538

G2X10.4334Y3.6883I.044J-.2062

G1X10.7091Y3.7311Z6.5594

G2X10.7208Y3.7326I.0324J-.2084

G1X10.9984Y3.76Z6.563

X11.297Y3.7894

G3X11.6314Y3.883I-.0981J.9952

G1X11.8568Y3.9911

Z6.663F33.

 

How could I cut the code length in half? Or can I? My Mazak doesn't take much G-code and this is only a small part of my program.

 

Any help would be great.

 

Thanks,

[HVC]

You can try filtering your toolpath.

[Guest CNC Apps Guy 1]

Filter????

 

Or if the program is too long use the "section" C-Hook. It cuts your programs inat a workable size.

 

HTJH

[HVC]

Yeah James i think you were the one who taught me how all the setting in filtering worked.

[Noel]

Will your control accept an r value in place of I and J you could change you post to output an r value.

 

 

Noel

[LFP]

I changed I and J to R, and put on my filters but still same amount of lines. I am a bit unsure what to do with the filter. Plus does the linerization tolerance and max. depth variance change amount of lines?

 

Thanks

[Lee.]

Hi there,

 

If you can slacken the filter tolerance that would for sure give you less lines. You just have to understand that the filter tolerance will let your cutter wander off the corect path to create arcs as long as possible before it will create another.

 

One other thing to watch is the minimum arc radius and the maximum arc radius. Make sure these are allowing the filter to do it's thing.

 

On the linearization tolerance that will increase yopur deviation some more. Say you have a lin tol of .0005 and a filter tol of .001, you essentially have an overall tolerance of .0015. If you can live with that then I say go for it. If yopu can stand more, then increase both.

 

HTH,

 

Lee.

[Lee.]

I wouldn't play around with changing the type of arc output, that should be left well alone. Your machine Control would determine which to use.

 

 

Another thing you could check in your post is, BRTEAKARC. cHECK TO SEE IF YOU ARE OUTPUTTING QUADRANTS OR ALLOWING IT TO DO FULL CIRCLES. tHIS WILL ALSO DECREASE THE AMOUNT OF CODE.

 

Sorry about the cap screw up.

 

Lee.

[LFP]

Getting smaller, what's the difference between the one way filtering option, on or off. breakarcs is set to 'no', what should it be?

[P_Scott]

LFP,

 

One-way filtering means the software will filter the cut when the tool is going in one direction of say, an alternating direction toolpath (ZigZag: filters Zig but not Zag). Looking at your original code I sense there will be a problem. The Filtering in Mastercam traditionally works best to replace many consecutive linear moves (G1's) with less arcs. Having arcs in between the lines is probably why the filter doesn't seem to be working the way it should. The software is confusing what's already there with previously filtered toolpath and doesn't filter any more because it seems redundant. Try the toolpath again, without getting rid of the first one, and see if there's any change when you apply the filter settings as you fill out the parameters of the second toolpath. HTH

[Dennis at CAD/CAM Consulting]

Your program looks like a simple 2D contour and that your chain contains multiple segments of lines and that the arc motion generated is the tool rolling over the corners or intersections of the lines...

 

On the Contour parameters page, Try setting the "Roll cutter around corners" option to "None". That should get rid of all of the arc moves, if they are not part of the chained geometry.

[BernieT]

+1 for Dennis

[Teh Bear without Brains kinda idiot]

If you would use cutter compensation ->control you would get better results for filtering

 

HTH

WTHH