Need Help!- Bobcad 21 - pocketing distortion

[buckey29]

I have Bobcad 21. I'm trying to do a very SIMPLE pocket.

I create a letter "A", then convert to verctors and pocket. The triangle in the center of course becomes an island.

I've tried this with 3 different fonts - all same issue.

Problem is that when I create the NC code, I seem to get an extra line of code that Bobcad inserts. That the top of the triangle (the island) or the lower right - it creates a circle.

One one I could see the issue clearly in the SIMULATE function. In another I couldn't see the problem until I tried to run it on my CNC Mill.

Is this a "known problem" Or am I doing something that could be causing this?


Addl Data: A - size 3.5, bit 1/4", step over .100, roughing pocket .25" deep in one pass.

Thanks for any thoughts or suggestions. Even if its a confirmation that its a known issue. COuldn't find any info on their site about it.

[tobyaxis]

Originally Posted by buckey29 I have Bobcad 21. I'm trying to do a very SIMPLE pocket. I create a letter "A", then convert to verctors and pocket. The triangle in the center of course becomes an island. I've tried this with 3 different fonts - all same issue. Problem is that when I create the NC code, I seem to get an extra line of code that Bobcad inserts. That the top of the triangle (the island) or the lower right - it creates a circle. One one I could see the issue clearly in the SIMULATE function. In another I couldn't see the problem until I tried to run it on my CNC Mill. Is this a "known problem" Or am I doing something that could be causing this? Addl Data: A - size 3.5, bit 1/4", step over .100, roughing pocket .25" deep in one pass. Thanks for any thoughts or suggestions. Even if its a confirmation that its a known issue. COuldn't find any info on their site about it.

Buckey29,

What your experiencing is called a Crop Circle. Your post processor is doing this and it can be corrected.

Open your file then the CAM side of the software. In the Main Menu on the CAM Side>Setup>General

Set the Max Circular Arc Movement according to what your machine can handle. If your not sure set it too Quarter. This will eliminate the Crop Circles.

One question I have is, "Are you using "I" and "J" or "R" Designations for Arcs"?

[buckey29]

Thanks for the response! That is what I love about these forums - people helping people. Bobcad called and asked me to open a "Support on demand" call. UGH.

I'll give that a shot. Just for reference I'm using Mach3 and the Mach3 postprocessor. The controller is HobbyCNC's distributed by Rual Routers (mikebeck.org).

How would I determine the Max Circular Arc for my machine? And what does that mean?

[tobyaxis]

Originally Posted by buckey29 Thanks for the response! That is what I love about these forums - people helping people. Bobcad called and asked me to open a "Support on demand" call. UGH. I'll give that a shot. Just for reference I'm using Mach3 and the Mach3 postprocessor. The controller is HobbyCNC's distributed by Rual Routers (mikebeck.org). How would I determine the Max Circular Arc for my machine? And what does that mean?

The Maximum Circular Arc refers to the maximum degree arc that your control is capable of making in a single move.

example:

O00001
G0G17G40G49G80G90M5
G91G30Z0M9
G90M19
M1

N1(EMILL 3/4D 1.5LOC 3FLT CBD)
T1M6
G90G54G40G0X0Y-.3S6000M3
G43Z1.H1
Z.1M8
G1Z0.F50.
G3X0Y-.3Z-.375J.375
Y-.3J.3
G1Y0.
G0Z.1M9
Z1.M5
G91G30Z0M19
G28Y0
M30
%


This short program will helix down to Z-.375 then in a full 360 degree circle spring pass to clean the lead on the helix.

These are the definitions

Full Circular Arc 360 Degrees
Half is 180 Degrees
Quarter is 90 Degrees

[buckey29]

Thank you for your reply and answer. I appreciate it!

[orizaba]

Toby, If Bobcad isnt paying you a LOT of money, they should be.

Not to torpedo this thread, but I have another question. (V22) I cannot post any of the 3D or 2D files. It worked great (I cut out two parts) until I tried to generate an Equidistant off set tool path. Now I get a "BOBCAD not responding" some of the time when I try to generate the tool path. When I do manage to get a tool path it dosent do anything when I ask it to post. What have I done this time?

Thanks Again
Matt

[tobyaxis]

Originally Posted by orizaba Toby, If Bobcad isnt paying you a LOT of money, they should be. Not to torpedo this thread, but I have another question. (V22) I cannot post any of the 3D or 2D files. It worked great (I cut out two parts) until I tried to generate an Equidistant off set tool path. Now I get a "BOBCAD not responding" some of the time when I try to generate the tool path. When I do manage to get a tool path it dosent do anything when I ask it to post. What have I done this time? Thanks Again Matt

All CAD/CAM when posting or processing G-Code looks that way in the Task Manager. I have no clue as to why, but they just do.

As far as getting paid by BCC, I wish. I would be able to retire at a young age LOL.

So unless your PC totally locks up, wait until it is finished processing. I have had tool paths take 3 hours to process because the parts were very big and the G-Code program around 1.5 million sequence blocks long.

PC's and Software are funny little things

[Claude Boudreau]

I get crop circles too
I cant find a General menu in the Setup menu (Cam side , Ver.21)

dont see Max circular arc movement anywhere...

[tobyaxis]

Originally Posted by Claude Boudreau I get crop circles too I cant find a General menu in the Setup menu (Cam side , Ver.21) dont see Max circular arc movement anywhere...

Claude Boudreau,

Open a new file, Click on the Milling Machine Icon or go to the Special/NC-CAM in the Main menu. You will find "Insert NC" choose a Machine Control Configuration like Fanuc6M Simple

Another window will open on the left side.
At the top in the Main Menu go to Setup then from the drop down menu select "Driver". Now go to the General Tab and toward the bottom you will see "Max Circular Movement" Full>Half>Quarter

Chose the one that your control is capable of doing.

Do not forget to Save the file as a blank file if you have no Drawing Opened.

[orizaba]

I had a little glitch show uplast night on a trial cut. In the middle of a large program I put in two pockets with a verticle entry. The pockets are in the wrong place, and it cut profiles with a lateral entry. I have checked everything, including deleting that part of the geometry and cam tree and starting from scratch. It cut it wrong again.
I switched to Z level rough and it worked fine.
The pocket cut is a port that gets a valve seat pressed into it. Is Z level finish as accurate as a pocket cut in this situation?
Matt

[The One]

"Crop Circles" are not a result of the Max Arc movement. These are generated for two reasons. I will tell you why and give you a solution for each below:

Case 1: Accuracy error
In this case what happens is there is an entity or entities in the profile that are smaller than the alloted decimal output for the control. For example an arc with a small sweep where the beginning is X0.12453, Y0.2526 and the end of the arc is X0.12449, Y0.25263. When the system generates the code it rounds these values to get it down to 4 decimals. Now you have an arc that begins and ends at the same location (full circle).

To correct these errors:
Click on File => Environment.
Click on the Defaults tab.
Change the General Accuracy to 0.0001" or 0.001mm.
Then click OK.


Case 2: Non-tangent Arc segments
In this case the system is generating an arc move around a corner produced at the intersection of an arc and line or an arc and an arc. This is done because the arcs are not tangent to the adjacent entities. Believe it ornot, this type of problem is the most common and is, more often than not, due to the part design and not the program.

To correct these errors:
Select the geometry used to create the toolpath (before the toolpath is created).
Then click on Change => Reorganize => Make Arcs tangential.
In the dialog the Max Acceptable Angle is the largest angle of deviation you will allow. I normally set this to .001.
The Max Angle for correction is largest angle of deviation you want to fix or make tangent. As you make changes the Number of Corrections to do field will be updated.
After clicking OK the corrections will be done and you should apply the toolpath.

This is more of an art than a science a lot of time, so you may need to play with it a bit to get it down to a science for your parts. But either of these cases, or even both, will resolve the issue with "Crop Circles".

Regards

[Claude Boudreau]

The One, you should be name The great One.
I`m on my knees in front of such wisdom.