Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: gm276 on August 05, 2007, 08:28:16 PM
-
I have just started using LazyCam Pro under vista (Mach3 2.4).
It's great! And for the most part really lets me get to what I need
to do quickly. Now for the confusion.
I created a dxf text letter in my cad program (designcad) .
I opened the DXF file in Lazycam. Everything looked great!
Then I pocketed the letter using .125 inch as my mill size.
Again all looked well.
I posted the G-code and flipped over to Mach3.
This is where it got strange. It looks like as it was doing
curves it tryed to do a small section of curve but instead
did a complete reverse circle.
Probably obvious but not to me. Any ideas.
Thanks
Don B
[i mg]
-
try running a smaller cutter it maybe that the tool is doing a postional move
-
The path looks fine in the LazyCam view.
See attachement.
I also tried smaller cutter 1/16
and still have problem
Don B
-
Looks like a rounding problem. I found five lines that had the same endind point as the previous line, but they were arcs with I's and J's.
That is a command to do a complete circle.
N3005 G2 X1.0123 Y1.3842 I-0.0019 J-0.0312
N3010 G1 X1.0189 Y1.3837
N3015 G2 X1.0189 Y1.3837 I-0.0024 J-0.0312
N3020 G1 X1.0254 Y1.3832
Line N3015 has the same end point as N3010. Also N3405, N4300, N4735, and N4765.
I'm sorry I can't help with Lazy Cam, I haven't had a chance to look at it yet, but if you want to fix what you have just delete the bad lines.
-
check the dxf to see that the lines join at the end poimt. Can you post a dxf of the cut out
-
Here is the dxf file of the cutout.
Thanks Don B
-
Your file worked fine in Bobcad here the code
-
Thanks for trying it in Bobcad. I put the bobcad file
in mach3 and it appears to get stuck. Attached is the
screen. See attachment.
-
Seems like you got the absolute and incremental settings screwed up in the General config setup! Then you will get circles where there shouldn't be any.
Try setting xy as abs and IJ as incremental. Or vice versa! Not sure which is which, I'll hav to check, but I think that's what you got!
Regards,
Whacko
-
Try this file I just ran it thru mach 3 off line and it seems to work. you need to set rpm and Z depth along with the feed you want
-
just to let you know that it is programed for 1/8 tool. if you want to add cutter comp you need to put the code and offsets in. There is no H,D,G ect
-
I'm still confused.
I tried the file.
Now I only see one corner where
this circle event happens.
I tried loading another computer (my laptop)
and I get the same thing.
thanks
Don B
-
Line 272 has no value for X which
makes X the same as existing and
a circle occurs. I edited line 272 to
include an X value different from the
existing value and the circle went away.
Don B
-
There is something funny about this geomitry. I did not zoom in close enought the first time.I think htere is an issue here let's look a little closer before you run or do an air pass first
-
What I found that the top side of that V has 66 line just to go acrossed. I reworked that side here some code and a dxf your file just went from 395 enities to 328 entities from just changing that one area
-
I have to agree the DXF file may overly complex.
I am noticing the same thing from some code
generated from Bobcad. It generates G2 moves
with out any X or Y value which seems to generate
a circle in Mach3. Thanks for your help. I think I'll do
some reading on the G2 and see if I can learn a bit more.
Thanks
Don B
-
I am guessing that due to the overly
detailed DXF, that the changes in xy
are too small sometimes to generate a different
x or y ( at least withing the preciision of the
current gcode.
Don B
-
This is a bug in Lcam... I am working on fixing it at this time :( The problem is the start and end of an Arc section is less then .00001 diff. So when the file is posted the numbers are rounded to be the same as the start point and this will give you circle. So in your Gcode file just delete the circle and the file will run okay. I will be fixing that bug tomorrow night.
Thanks
Brian
-
Brian,
You made my night!
Thanks to all for the input.
Don B
-
check the dxf to see that the lines join at the end poimt. Can you post a dxf of the cut out
Brain amd GM276 This was my first thought. In Bobcad we call the crop circles. But what happens is the software is making a position move from the end of one line to the start of the next.
Here is a post from the bobcad forum by the Bird BCC tech. man
Believe it or not, the crop circles that most people get are due to the geometry used to generate the toolpath.
What happens is when you have an arc and a line that intersect and the line is not perfectly tangent to the arc, the system generates an arc move around the corner. This arc can be so small that the beginning and end of the arc have a difference that is less than 0.00005, so when the coordinates are rounded you get the same position for both the end of the arc and the beginning of the arc (full circle).
I suggest trying to use the Make Arcs Tangential command, when possible. That alone should help reduce the appearance of the arcs.
Regards
-
When downloaded that file looks like a spline that has beeen exploded in autocad. Hundreds of short segments end to end. (;-) TP
-
Vmax,
I would not be surprised. This file was generated
in DesignCad using a truetype font and saved
in vector format. (option in Designcad)
It was then exported to be a DXF file before being
read by LazyCam.
Don B
-
It may not have been a bug in lasycam. I have never used lasycam but if you imported the file that where your issue is.Autocad and other drawing programs are great for drawing.But arc and ellispes done in these program are allway trouble.Autocad is one of the worsed programs for cam system to use.It not the software but the people that draw with it don't see these issue as they don't machine them generaily. So when they draw they just use poly-lines. There is a command in autocad to change out of polyline. But I don't known what it is as it been years sence I used Autocad. Some like Ger21 would know as he is a Autocad expert
-
Been using Acad for years never had any trouble with cam issues. You just have to remember that CNC machines tend to think in limited terms. Draw it like you were going to machine it. Make sure that your lines and arcs actually connect( most errors tend to occur here). Never had any trouble with polylines???? Must have been lucky. Have noticed that the more times you wash the original file through interpetive programs the more that file degrades as far as line quaulity and line interpetation.
(;-) TP
-
The problems should be fixed in the next rev (I seem to have fixed them here that is) I also have my first stab at tabbing done ! So you can tell me how that is working as well :)
Should be out at some point Monday
Thanks
Brian
-
Never had any trouble with polylines????
(;-) TP
Mach does not seem to have any issue with polylines. In some machine polyline will raise hell. If you have look a head. In a Fedal I ran we used to turn it off just so it would be a smooth motion instead of starting and stopping
-
I had the same problem on a drawing I did with corel draw, when I performed offsets with Lazy cam. No indication as to where the circles came from. I just removed the unwanted code. Strange that in lazy cam there was nothing on the drawing to indicate the unwanted circles. It wasn't until I pulled it up on mach3 that I saw the problem.
Another trick I was told was to zoom in on the drawing before offsetting. Not sure why, but it does help in improving the offsets. I am finding offsetting to be a little frustrating at times. I am sure there must be a glitch in the program. Sometimes lazy cam wont offset at all, which is aggravating because you have no indication of why it wont. So you sit and wonder if its the user or the program. One day I just kept hitting the offset button over and over. Then around the 20th or so time, it created an offset.........I did nothing more then just hit the button.
-
I've noticed an interesting occurance with offsetting. If you move the "arrow" showing the direction of cut on a particular chain, to a new spot, it will magically offset with no issues. :)
-
Yes, I have used the "moving the arrown to a new position" will sometimes get the offset to create. Another trick is to rotate the drawing, do the offset, then rotate back. Man, what a guy will try when desperate for an offset.
-
Hi, Dave & Jonny
I've had these Cir. from nowhere at times to deal with also, Reorienting, editing them out in Mach after posting.
As far as Tricks and things to try, Someone (Sorry I don't remember who) suggested that after you load your dxf and clean & optimize it, Post it to Mach then, Use the "Mach3Load" Button/feature in LazyCam to retrieve it back from Mach and use it to do all your modifying and then re-post.
I've had some success with doing this with problem drawings, Give it a try.
Thanks, Chip
-
Thanks, Chip and Jonny, you can never have too many tricks up your sleeve- :)
-
Hi Guys, Instead of inserting hundreds of line of Gcode into a thread. Please just upload it as a text file.
Thanks.