CAMheads CNC Router Forum By: CAMaster CNC

Go Back   CAMheads CNC Router Forum By: CAMaster CNC > Software > BobCAD-CAM

Reply
 
Thread Tools Display Modes
  #21  
Old 02-24-2014, 07:28 AM
tchapman tchapman is offline
CAMhead Friend
 
Join Date: Feb 2014
Posts: 39
Default

Looks like to try the nest demo, you have to install the entire V26 demo, I had to put it on another laptop since it seemed like it had a conflict with installing on a laptop with licensed version. The nesting feature has a tab feature built in that is exactly what is needed, it will select any number of tabs or you can pick points. There is a way to turn off the nesting features to avoid it creating copies by deselecting "active" parts button. There is a default profile that is created that can be edited which will apply it's rules to all the parts. It also creates individual profiles for each part, these can be edited separately or revert back to the default. The tab multi pass image shows the effect of 2 passes, with examples of different tab placements and heights. I think that plan is to use the nesting option for the final route of the parts. This is pretty simple after a few minutes of practice.
Attached Images
File Type: jpg nest.jpg (25.4 KB, 12 views)
File Type: jpg nest2.jpg (37.0 KB, 14 views)
File Type: jpg tab with multipass.jpg (77.6 KB, 9 views)
__________________
Stinger 1 + Wincnc
Bobcad V20, V26
www.dadodoor.com
Todd Chapman

Last edited by tchapman; 02-24-2014 at 08:35 AM.
Reply With Quote
  #22  
Old 02-24-2014, 08:54 AM
aldepoalo aldepoalo is offline
CAMhead Legend
 
Join Date: Mar 2011
Location: Clearwater FL
Posts: 118
Default

"Al, when you have a chance, can you please let me know how to fix this. Using the toolpath in an array or as translated, each feature behaves well until it gets to a new feature. When it leaves that current feature move, it raises to the correct rapid but the tool begins moving towards the first z height in the next feature toolpath, which means it starts diving into the surface before it gets to the correct position. I have been correcting this by taking the posted file, going into edit, doing a find for "[" which goes to top of each new feature to allow easy tweaks. The first line of each new feature is a G01(pocket or rough), with Z sitting below 0. So I add a new line with G0 at the same X and Y of the G01 line, but put Z at rapid. This fixes the dive. Is this a problem with the post or with V26?"

This would be a post issue:

When the tool moves between features the code should look something like this:


N34 G00 Z0.2
N35 Z1.

(NEXT CUT - SAME TOOL)
(JOB 1 Profile Finish)
(PROFILE FINISH)

N36 X0.375 Y0.375 S1191
N37 Z0.2


Where the tool moves up.
The it moves over in X & Y to the next start
Then it moves down for the next cut.

************* 50 - Rapid moves//Rapid move Z **********
N35 Z1.
************* 4 - Tool Change//Move to next cut same tool **********

(NEXT CUT - SAME TOOL)
(JOB 1 Profile Finish)
(PROFILE FINISH)

N36 X0.375 Y0.375 S1191
************* 40 - Operations//Start of operation **********
************* 50 - Rapid moves//Rapid move Z **********
N37 Z0.2


4. Null tool change
" "
"(NEXT CUT - SAME TOOL)"
system_comment
feature_name_comment
" "
force_no_add_spaces
output_rotary_angle
output_second_rotary_angle
default_add_spaces
n,rapid_move,force_x,xr,force_y,yr,p_rot, s_rot,s


The rapid move with force positions on the post you are using would need to be changed so the there is no z on that line.

Can you tell me which post you are using? Is it the one off off wincnc website?
__________________
Al DePoalo
Partner Products Manager
BobCAD CAM, Inc.

Last edited by aldepoalo; 02-24-2014 at 09:17 AM.
Reply With Quote
  #23  
Old 02-24-2014, 09:00 AM
aldepoalo aldepoalo is offline
CAMhead Legend
 
Join Date: Mar 2011
Location: Clearwater FL
Posts: 118
Default Tool Stay Down:

"Next issue. Using a rough pocket, I want the tool to cut the first depth, the move directly to the next step down. As is, the tool moves up to rapid Z first before moving to the next depth. This will save a lot of time on a large panel. I tried the option to spiral down, the simulation looks fine with the spiral toolpath showing below Z. However, in Wincnc, the tool moves to the surface at Z0, then does a number of arcs representing the spiral, but never moves below Z. Looking at the code, there is no reference to the actual Z depth that was specified. This does not make sense when the sim works fine and the toolpath is clearly visible below Z from side view in the main view. Somewhere, the Z depth is getting lost in the output and never makes it to the file. I have tried both the 'new' wincnc posts. I think the spiral type plunge will accomplish the goal but if there are other ways please advise."

Currently we do not offer a Tool stay down option. So that means the tool will go to clearance after very increment of cut.

So you can choose to ramp down instead. You can post with line moves or arc moves which is set by both the post and the UI for the feature you are using.

What I would recommend is using a profile with contour ramping. Where you either ramp to to full depth and cut around the shape, or where you ramp down at a given angle or increment till you get to the final depth.

You can post with lines moves if your controller doesn't support helix moves, or you can post with G02/G03 moves that have Z values.

Again if the post you are using doesn't have the Z value in the code the post will be need to be updated.

The one on wincnc's website was written I think 1 or 2 years ago, so it could use an update and I would be more than willing to help dial it in with ya.
__________________
Al DePoalo
Partner Products Manager
BobCAD CAM, Inc.
Reply With Quote
  #24  
Old 02-24-2014, 09:37 AM
tchapman tchapman is offline
CAMhead Friend
 
Join Date: Feb 2014
Posts: 39
Default

Thanks Al

http://www.wincnc.net/webfiles/Post%...essors/BobCAD/

I am using either of the NEW posts here, no difference that I can tell. If you think of any improvements, please let us know.

I just bought nesting so that should solve the tab requirements very nicely. I see a feature in the tabs for the cutout not sure why this always computes in the same toolpath as the tabbed toolpath, sort of defeats the purpose to include the tab toolpath in the same output as the cutaway? I see no way to separate the tab from the cutaway feature. I would want the cutaway toolpath to be a separate toolpath that can be posted separately and ran after all the tabs are created.
__________________
Stinger 1 + Wincnc
Bobcad V20, V26
www.dadodoor.com
Todd Chapman
Reply With Quote
  #25  
Old 02-24-2014, 09:46 AM
aldepoalo aldepoalo is offline
CAMhead Legend
 
Join Date: Mar 2011
Location: Clearwater FL
Posts: 118
Default Post Edit:

Ok so I downloaded the first post and just like I thought the null tool change block is missing some codes.

4. Null tool change
system_comment
feature_name_comment
output_rotary_angle

This block should have an X and Y move to force the tool to move to position at clearance and to remove the "ramp" move that you got that is creating scrap for you...

So I can fix that easy...

What other changes do you feel are needed?
__________________
Al DePoalo
Partner Products Manager
BobCAD CAM, Inc.
Reply With Quote
  #26  
Old 02-24-2014, 01:57 PM
tchapman tchapman is offline
CAMhead Friend
 
Join Date: Feb 2014
Posts: 39
Default

Thanks for looking at this.

The only thing that I would love to have an option for is when I know I am making a file with no tool changes, it would be nice to know how to make post that does not include the T1 near the top. As it is, I have to manually go in to comment out the line per file. Can an simple edit to the post be made so it has NTC ( no tool change ) designation in the post name?

On a side note, I wish you could look at the tab feature in nest add on. It has a button called cutout, that adds in the little piece that was removed. However, the little piece is included in the same toolpath as the tabbed toolpath. What is needed is a way to create a file for the tabbed toolpath, run that file, pause or go to a new file that ONLY contains the small piece for cutting the tab out. I want to leave a robust tab while the machine is unattended. Then, load a file and run it attended, hand hold each piece as it is cut loose. Maybe you know a way to do this but as is the button for cutout doesn't make sense. Heck, maybe I will just make a smaller tab and break it by hand and forget the cutout.

I called your tech support after buying the nest for tab purposes, they suggested the tab is not designed to work how I am trying to do it. But, with some tweaks it works perfectly. If anyone is interested I will post the method that allows the nest to create the tabs, but leave everything else perfectly in place so the geometry lines up with the original parts.
Attached Images
File Type: jpg photo.jpg (42.8 KB, 23 views)
__________________
Stinger 1 + Wincnc
Bobcad V20, V26
www.dadodoor.com
Todd Chapman
Reply With Quote
  #27  
Old 02-24-2014, 10:05 PM
richf richf is offline
Cobra Owner
 
Join Date: Apr 2011
Location: New Hampshire
Posts: 780
Default

Great idea on the tab trimmng. I've never investigated the nesting addon. I didn't realize it had options for creating tabs. I wouldn't mind hearing a summary about your technique to make it work.
__________________
Rich F.
PrecisionSignandPost.com
CAMaster Cobra 408 X3 w/Recoil
BobCAD v25 4th Axis
Corel Draw X5
Reply With Quote
  #28  
Old 02-25-2014, 08:44 AM
tchapman tchapman is offline
CAMhead Friend
 
Join Date: Feb 2014
Posts: 39
Default

Rich, here are my notes. If you have any questions let me know.

1. Create parts to machine inside a box with lower left corner of box at 0,0. The outter box that represents your actual machine coordinates and should match the panel you have loaded. Note: It may work by putting a laser on the lower left corner of material or your start position of work at 0,0 using a set point for 0,0 other than machine. The Sheet MUST be larger than that outter box you are working with.
2. Have all the outside final route geometry inside the large box. It is best to use a new file in Bobcad so you can see the tabs and check for alignment at various angles without other lines in the way.
3. Make the stock show the material size as .1 x .1 x .1 just to make it go away, it keeps the main work area more visible.
4. Select in cam defaults New nesting Job.
5. in Nesting job, click select geometry. Drag mouse over everything. Right click OK.
6. Go through each setup screen. Leave most as is, but change:
Rapid Height
Check Generate Toolpath before nesting
Check Conventional MIll
Uncheck Rotate
Change stock margine to -0.01575 (this will round to -.0158 but it makes a difference to start with 5 decimals.)
Check Nest Quantity before proceeding

In tabs page, check Part ID, and anything in the list below. Check apply tabs and tabs on inner profile. Enter number of automatic tabs you want. Enter width of tab ie .35". Change height of tab ie .025". Uncheck Add Tool Diameter. Uncheck Create Cutoff Feature.

In the Data Cam tree, you will now have an Outter Profile plus a number of inner profiles based on how many parts you have inside the outter profile. I do not suggest you change any of the individual sections. You can edit the Default profile as needed and recompute as you need.
Right click Nesting Job, select compute toolpath. View the result and see if the green lines representing the tool path is A. on the inside of the outter box, B. on the outside of each inner box(part). If not, then go to the default profile, hit edit, go to section to change from Left > Right and reverse it. Hit compute again to see the change. When correct, the outter box will have the green on the inside, and the part geometry will have the toopath(green) on the outside of each part. I would not try reversing the direction of each part.

Notes:
The nesting/tab feature is quirky:
If you change a tab height or width, you must FIRST recompute, then go to Nesting Job>Edit>Parameters and change convention mill to climb. Hit recompute. Then go put it back to conventional, hit recompute again to actually see a result of the tab change.
If you want multiple passes to cut the part out, edit in Defauly Profile, select multiple passes and adjust your max depth. Recompute. If you do not see a change, change to Climb, recompute, change back to conventional, then recompute.
Custom Tabs: This has been buggy. Sometimes it will get so weird that it is best to start over. I have seen it show the tab but also show the cutout all the way to the bottom. I have entered all new custom tab points, only to see it still show the original, and would never show my edits. Use automatic tabs when possible. I have not had luck with manual tab entry. This is very buggy.
If you do not see any tabs after computing, try toggling the climb>conventional modes as desribed and compute each time. If the toolpath is on the inside of the part geometry, it will sometimes not show the tabs but shows cut all the way to the bottom.
The offset of -.0158" is required to put the geometry back to where it should be, this is within .0001 of the original. If you zoom in to 0,0, you may see that there are actually 2 blue outter boxes stacked on top of each other. Zoom in enough and you will see that there are not perfectly stacked. However, if you enter the offset -.01575" ( 5 decimals), it will pull it much closer upon compute. However, after you type in -.01575, the displayed value reverts to 4 decimals, EVEN THOUGH the behavior actually works using 5 decimal places. Keep in mind, it is unlikely your part will care about a .0001" deviation. on the outside.

Before posting, tell the Outter Profile not to post.

It may be needed to go to Cam Tree, click on Part 1 ( or 2 or 3 etc) under Machine Setup, delete, then reselect geometry, recompute. Your Default Profile and tabs should be the same.

If the tab height does not change after toggling climb>compute, conventional compute, then delete the Part, reselect geom, compute.


Once you practice a few times, this all gets easy and it works great. I have yet to solve what the cutoff option does, I would like it to create a separate profile and toolpath just to cut that length, but instead it just cuts the entire part to the bottom, not useful.
Attached Images
File Type: jpg tabs2.jpg (80.5 KB, 6 views)
File Type: jpg tabs.jpg (20.5 KB, 7 views)
__________________
Stinger 1 + Wincnc
Bobcad V20, V26
www.dadodoor.com
Todd Chapman

Last edited by tchapman; 02-25-2014 at 09:46 AM.
Reply With Quote
  #29  
Old 03-02-2014, 11:11 AM
richf richf is offline
Cobra Owner
 
Join Date: Apr 2011
Location: New Hampshire
Posts: 780
Default

Great write up and certainly well above a summary. Did you happen to read of the Bobcad documentation related to nesting first or strictly go by Al's video and directions?

I won't be able to replicate because I don't have nesting but this is great reference for the future. I'll look into the nest option when the business need arises. I still like your idea of coming up with a toolpath containing only the tab profiles only so they can be cut separately. I might play with that option in the future.
__________________
Rich F.
PrecisionSignandPost.com
CAMaster Cobra 408 X3 w/Recoil
BobCAD v25 4th Axis
Corel Draw X5
Reply With Quote
  #30  
Old 03-02-2014, 12:38 PM
tchapman tchapman is offline
CAMhead Friend
 
Join Date: Feb 2014
Posts: 39
Default

In terms of the nesting, I didn't watch any vids, since I am not really "nesting", I am only using the tabs, so I didn't bother. I am now using the nesting feature in the same file versus creating a new file, simpler and less files to keep track of. Same concept as above. The nesting job can only be posted separately, I have not seen a way to post both a mill job and nest job into one file, but I prefer separate. I learned to create 3 tabs, at full height, .01" wide. This works perfectly and parts snap out with a breeze, just a small predictable tab to sand off. Before I was using a short height tab but .25" wide, much more unpredictable and more effort on clean up since it produces more onion skin.

You could haggle with BC and not pay retail, and to me it is worth the money. But, in reality you can create a contour, put in an arc on several entities, quick trim and get the same result, just more work if you have a lot of different parts on a panel.
__________________
Stinger 1 + Wincnc
Bobcad V20, V26
www.dadodoor.com
Todd Chapman
Reply With Quote
Reply

Thread Tools
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

Forum Jump


All times are GMT -4. The time now is 10:55 AM.


Powered by vBulletin® Version 3.8.4
Copyright ©2000 - 2018, Jelsoft Enterprises Ltd.