CNCzone.com-The Largest Machinist Community on the net!



Home Page Mark Forums Read Today's Posts My Replies Classifieds Reviews Photo Gallery Web Links Share Files Advertise With Us Ad List
Go Back   CNCzone.com-The Largest Machinist Community on the net! > CAM Software > SprutCAM


SprutCAM Discuss SprutCAM software here.


This forum is sponsored by:

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #1   Ban this user!
Old 01-08-2011, 01:03 PM
 
Join Date: Mar 2010
Location: USA
Posts: 816
Magnum164 is on a distinguished road
SprutCam Defaults

Looks like I am still having problems with metric/imperial in my machine. Need to get some input from everyone. The other day I was machining some pockets and everything was well, but the rapid down into the material was very fast and hard. I let the machine run as the bit would have broke the first time if it was going to break. Later I realized that the force had actually flattened the center cutting tips and it showed when I machined the top surface.

Checking SC, it seemed everything was fine, till I went to the rapids feed menu. I realized it is not set as a percent of the work feed and not sure why it's not. Mine always defaults to 394 in all processes.

Just curious if anyone else has noticed this as being 394. I just entered 3 as a start and the rest of the parts cut fine with no harsh rapid plunging in the pocket.

I like SC, but i don't like having to check all of these menus. You would think if the rest are a percent of the work feed the rapids should default to a standard percent as well. I have a feeling the 394 is metric, converting it over would be about 15IPM which would have been a little reasonable but still to fast for my .125 EM.
Attached Thumbnails
Click image for larger version

Name:	sprutcam_menus.jpg‎
Views:	47
Size:	45.7 KB
ID:	123389  
Reply With Quote

  #2   Ban this user!
Old 01-09-2011, 01:07 AM
 
Join Date: Jun 2006
Location: Australia
Posts: 139
bevinp is on a distinguished road

You may be able to set the default parameters by modifying the .xml files. Eric produced a training video last year showing how to make changes to certain default settings in those files. When I changed my files, I noticed one of those files also listed default speeds/feeds, can't remember which. Might be worth a look.
Bevin
Reply With Quote

  #3   Ban this user!
Old 01-09-2011, 08:27 AM
 
Join Date: Mar 2009
Location: U.S.
Posts: 44
Eric_Tormach is on a distinguished road

One of the most important issues discussed when I visited SprutCAM was that the values that they put as default, in many different areas are wrong. It took some explaining to get across to them that a default that is wrong might as well be 0, or blank, then at least we lessen the possibility of a destructive value such as you have. In order for me to effectively catalog and present these issues to SprutCAM it would be helpful, that when people come across these problems that they send me an explanation and let me know what build and rev they are running. This way I can make a bug report to SprutCAM.
Reply With Quote

  #4   Ban this user!
Old 01-09-2011, 08:46 AM
 
Join Date: Mar 2009
Location: U.S.
Posts: 44
Eric_Tormach is on a distinguished road

Also, as a side note, if the "Safe level" is set correctly then you should never rapid down into the material. You may want to also check your approach, and plunge feed rate. The "safe level" is the level in which the cutter will rapid to (it should be sufficiently above the work surface I usually use .05). After that safe level, the cutter will move at a feed rate (usually 50 percent of work feed). If instead of safe level a "safe distance" is used, you can find that the cutter may rapid into the material as "safe distance" is a incremental value.
Reply With Quote

  #5   Ban this user!
Old 01-09-2011, 01:54 PM
 
Join Date: Mar 2010
Location: USA
Posts: 816
Magnum164 is on a distinguished road

Originally Posted by Eric_Tormach View Post
One of the most important issues discussed when I visited SprutCAM was that the values that they put as default, in many different areas are wrong. It took some explaining to get across to them that a default that is wrong might as well be 0, or blank, then at least we lessen the possibility of a destructive value such as you have. In order for me to effectively catalog and present these issues to SprutCAM it would be helpful, that when people come across these problems that they send me an explanation and let me know what build and rev they are running. This way I can make a bug report to SprutCAM.
I generally try and make sure there is not something I am doing wrong before I officially submit something. I can send you some info later today.
Reply With Quote

Sponsored Links
  #6   Ban this user!
Old 01-09-2011, 01:59 PM
 
Join Date: Mar 2010
Location: USA
Posts: 816
Magnum164 is on a distinguished road

Originally Posted by Eric_Tormach View Post
Also, as a side note, if the "Safe level" is set correctly then you should never rapid down into the material. You may want to also check your approach, and plunge feed rate. The "safe level" is the level in which the cutter will rapid to (it should be sufficiently above the work surface I usually use .05). After that safe level, the cutter will move at a feed rate (usually 50 percent of work feed). If instead of safe level a "safe distance" is used, you can find that the cutter may rapid into the material as "safe distance" is a incremental value.
To me I see this as the problem. I always use a safe level of .1 (since all my parts are made from .25 plate) and since that is what the training videos show. Today I changed and used a safe distance of about .035 and it does feed harder as you mentioned.

If there is a difference in how the feed is determined by selecting these two options then the software should somehow alert the user. I would not think changing the distance the cutter starts would have an impact on how fast it feeds.

At least by setting the value to 4 I have not had anymore flattened end mills
Reply With Quote

  #7   Ban this user!
Old 01-09-2011, 03:36 PM
 
Join Date: Mar 2009
Location: U.S.
Posts: 44
Eric_Tormach is on a distinguished road

I'm sorry if you misunderstood my points from the previous replies. The cutter will not "feed harder" ever. There are two setting to be aware of. One is "safe level" this should be set to a point above the part (normally a Z+ amount) some of my videos show .1 and some .05 depending apon the mood I am in when I make them. The safe level is the level that it is safe for the cutter to move at a rapid rate to the hight specified. After the cutter has reached this level a G1 with a feed rate value is used to feed the cutter into the part. The feed rate value for the initial cut down into the part will be the "approach feed" You must select the value you want either by designating a % of work feed or giving it a value of it's own. I am willing to bet at no time in your G code that there was a feed rate value of 394. Please post your G code for analysis. The other feed rate you must consider is plunge rate, and you must select a value in the same way you selected a value fro approach feed. In order to understand where these values occur in the G-code I recommended putting in strange values (.123-.567) then looking at the G-code so you know where these occur (see attached picture). I hope the picture clears up any issues. Remember it is always important to review the G code. I don't know of any CAM software that will warn a user that their programmed feed rates are incorrect.
Attached Thumbnails
Click image for larger version

Name:	settings.jpg‎
Views:	42
Size:	268.1 KB
ID:	123479  
Reply With Quote

  #8   Ban this user!
Old 01-10-2011, 02:00 PM
 
Join Date: Mar 2010
Location: USA
Posts: 816
Magnum164 is on a distinguished road

Originally Posted by Eric_Tormach View Post
I'm sorry if you misunderstood my points from the previous replies. The cutter will not "feed harder" ever. There are two setting to be aware of. One is "safe level" this should be set to a point above the part (normally a Z+ amount) some of my videos show .1 and some .05 depending apon the mood I am in when I make them. The safe level is the level that it is safe for the cutter to move at a rapid rate to the hight specified. After the cutter has reached this level a G1 with a feed rate value is used to feed the cutter into the part. The feed rate value for the initial cut down into the part will be the "approach feed" You must select the value you want either by designating a % of work feed or giving it a value of it's own. I am willing to bet at no time in your G code that there was a feed rate value of 394. Please post your G code for analysis. The other feed rate you must consider is plunge rate, and you must select a value in the same way you selected a value fro approach feed. In order to understand where these values occur in the G-code I recommended putting in strange values (.123-.567) then looking at the G-code so you know where these occur (see attached picture). I hope the picture clears up any issues. Remember it is always important to review the G code. I don't know of any CAM software that will warn a user that their programmed feed rates are incorrect.

Well really never said that mine had 394 in it, I was more curious if this setting really affected anything.
Reply With Quote

  #9   Ban this user!
Old 01-11-2011, 04:19 PM
 
Join Date: Sep 2005
Location: USA
Posts: 366
RTP_Burnsville is on a distinguished road

Originally Posted by Eric_Tormach View Post
One of the most important issues discussed when I visited SprutCAM was that the values that they put as default, in many different areas are wrong. It took some explaining to get across to them that a default that is wrong might as well be 0, or blank, then at least we lessen the possibility of a destructive value such as you have.

Yes, I totally agree that no value is many times better than a wrong value. Please continue to stress that issue with SC.

Thanks,
Robert
Reply With Quote

  #10   Ban this user!
Old 01-11-2011, 05:03 PM
 
Join Date: Jun 2006
Location: USA
Posts: 980
MichaelHenry is on a distinguished road

Ditto to what Robert said.

Eric, I think that all of us appreciate you acting as a laison with SprutCAM. That can only help the program work better for us.

Mike
Reply With Quote

Sponsored Links
Reply




Currently Active Users Viewing This Thread: 1 (0 members and 1 guests)
 
Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Changing Defaults in SprutCAM cgroves Tormach PCNC 16 06-19-2010 11:46 PM
set defaults in SW 2008 Les George Solidworks 1 02-07-2010 07:57 AM
X4 Operation Defaults WingNutz Mastercam 4 12-31-2009 09:29 AM
Changing defaults in v9 juxtoposed Mastercam 4 12-08-2009 08:37 PM
Problem- Preadator 7.0 defaults orizaba BobCad-Cam 2 06-06-2008 10:38 AM




All times are GMT -5. The time now is 06:11 AM.





Powered by vBulletin® Version 3.8.7
Copyright ©2000 - 2012, vBulletin Solutions, Inc.
Content Relevant URLs by vBSEO
Template-Modifications by TMS

1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50 51 52 53 54 55 56 57 58 59 60 61 62 63 64 65 66 67 68 69 70 71 72 73 74 75 76 77 78 79 80 81 82 83 84 85 86 87 88 89 90 91 92 93 94 95 96 97 98 99 100 101 102 103 104 105 106 107 108 109 110 111 112 113 114 115 116 117 118 119 120 121 122 123 124 125 126 127 128 129 130 131 132 133 134 135 136 137 138 139 140 141 142 143 144 145 146 147 148 149 150 151 152 153 154 155 156 157 158 159 160 161 162 163 164 165 166 167 168 169 170 171 172 173 174 175 176 177 178 179 180 181 182 183 184 185 186 187 188 189 190 191 192 193 194 195 196 197 198 199 200 201 202 203 204 205 206 207 208 209 210 211 212 213 214 215 216 217 218 219 220 221 222 223 224 225 226 227 228 229 230 231 232 233 234 235 236 237 238 239 240 241 242 243 244 245 246 247 248 249 250 251 252 253 254 255 256 257 258 259 260 261 262 263 264 265 266 267 268 269 270 271 272 273 274 275 276 277 278 279 280 281 282 283 284 285 286 287 288 289 290 291 292 293 294 295 296 297 298 299 300 301 302 303 304 305 306 307 308 309 310 311 312 313 314 315 316 317 318 319 320 321 322 323 324 325 326 327 328 329 330 331 332 333 334 335 336 337 338 339 340 341 342 343 344 345 346 347 348 349 350 351 352 353 354 355 356 357 358 359 360 361