Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: stevehuck on September 01, 2009, 08:22:57 PM
-
Is it possible to take 4 entities out of a chain and create a new chain of those 4 entities. In the uploaded photo there is a thin strip that needs to be broken away from the outer chain.
Can this be done?
-
If I recall correctly, you can't do much at the entity level. You can delete them.
RICH
-
I think IF you start BEFORE you optimise the file it might can be done. If you upload the dxf file I will give it a whirl and let you know.
(;-) TP
-
Hi, Steve
Post your dxf as "TP" stated, You can also try changing the Setup, "Load Options" as shone in pic below,Then re-load the dxf and re-pocket it.
Chip
-
I have tried alot of things described above. No matter what i click that "rib" seems to always be part of the larger oval. All i want to do is pocket inside the big oval .032 deep and everything in there will be islands. Then i need to cut the outer oval to complete the part.
Here is the file
-
When I bring the drawing into Lcam those items ARE separate chains???? Not sure what you are doing to combine them. I used a line connect tolerance of .001"
(;-) TP
-
Not sure what you are doing to combine them. I used a line connect tolerance of .001"
(;-) TP
That was it!! I set mine to .001 also and BOOM! it worked!
Thank you!! Thank you!! Thank you!! Thank you!!
Steve
-
Now see if you can pocket the inside of the large oval and leave all those ribs. I think that large cluster in the center is too complicated. LC wants to machine the entire center removing all the ribs.
-
I am only guessing, but assume you want the ribs machined into the surface of the plate and then in the square part on the air cleaner you will put some text.
Adjust the spacing of the ribs to suite the tool you will use and the look you want to machine into the plate. For example; The current path spacing is about .030".
Create a pocket such that the pathing would be spaced bigger and actualy use a smaller tool adjusting the depth to suite what affect you want. You will need to lay it out some before hand.
Once you have the pathing you can assign cut parameters as you want.
But as i so state in the manual, you figure out what you want to machine before hand and don't try to use LC as a CAD program. ;)
RICH
-
Steve this part is TINY is it to scale??? IF so you will have to work with extremly small bits to make it work.
UNLESS that is the idea (;-) TP
-
Steve this part is TINY is it to scale??? IF so you will have to work with extremly small bits to make it work.
UNLESS that is the idea (;-) TP
This part is huge compared to some things i have made. I have a steam/air engine that has a .0625 bore and stroke and a .250 flywheel.
The first picture is the air cleaner i am trying to replicate. The second is the engine it has to fit. If the size is .950 wide and 1.950 long then it is to scale. The plan is to cut it out with a .016 end mill. This is the second project i am attempting to do with LC. The first went well but this one is giving some trouble but that's how you learn.
I tried to pocket the area but it did not leave the ribs as islands. It pocketed the entire oval. The tool being .016 and an overlap of .007 I thought would do the trick. Then i tried to do an offset around all the ribs in the center and it would only do a few ribs and stop. The offset would not go all the way around all the ribs in the center cluster. It is pretty complex but if you folks think it is possible, i will keep at it!
-
OK NOW I got ya, I'll work on it at that level then. I might be able to get it working now that I know the real scale of things.
(;-) TP
-
OK NOW I got ya, I'll work on it at that level then. I might be able to get it working now that I know the real scale of things.
(;-) TP
Keep track of what you do. The only reason for making this thing was to learn how to use LC and Mach3.
Thanks for all the help thus far!!
Picture of the steamer!
Steve
-
hi steve
here is a l-cam file and a pic. i scaled you up 16 to 1 in l-cam and and moved chains to new layers. used a scaled up tool wich comes out to .250
it generated paths ok. lcam does not like small stuff, so go big to go small. you have two options from here after generating paths. export the code scaled up and set the scale in mach3.or scale lcam back down after pathing then generate code.
bill
-
Hi Doc!
Thats some nice work there but.... Its backward. Take a look at the photo of the air cleaner about 4 posts ago. The part you cut was supposd to be the part that sticks up.
Sorry if i wasted some of your time.
-
steve
i did not target your part to cut it out. just trying to show you a possible solution to using l-cam. only wasted 5 min anyway.
that is a good l-cam file i gave you back ,you should be able to do alot of damage with it.
bill
-
forget this,sorry
-
You'r killing me!!
How exactly did you do that. I scaled up 20X and created a tool 20X and tried to do exactly what is in the previous post and no luck. Still wants to cut the entire oval out. Yes i checked "create islands" Is there something else in the setup stuff i need to change?
-
Hi, Steve
I used Bill's LCam file and used the .250 cutter for the tool, Are you using the Great Island's option as in pic 1 also selecting the chaines as in pic 2.
Hears a LCam file too look at, You will need to setup all the depths of cuts and move Chines around also.
Chip
-
STEVE,
Here is a different approch ( as i show and talk about in the manual ) for your air cleaner.
I have broken it down into machining steps, namely:
- Border
- Inside paths
- engraving area
- drilling
In this way you have complete control over what you want to do and there is no problem with the code generation into Mach. The pathing inside will leave a raised portion .016" wide and assume that on the path you will cut .016" deep. Would cut the inside border with a square .016" end mill.
Oh, btw, it's .975" wide x 1.950" long and i hope your machine cuts accurately or it will look crappy!
RICH
-
Hi Steve
you aint dead yet, here is another pile of crap. heheheh!
you said you are going to use a .016 cutter ,so i guess the real number is .015625 . at 16 to 1 that moves up to .250 . the l-cam i gave you was allready pumped up 16 t0 1 ,your orignal dxf imported showed X as 1.950 ,bumped to 16 to 1 made X 31.200 .
the first thing i do after loading a file into l-cam is to turn leds off then turn the rapids off before doing anything. maybe that might be causing you a little snag. those two items mess the chains real bad.you dont need them until the end.
i made two g-codes for you that cut .016 deep so if you want to try to run them make sure to edit the feed and speeds.these tool paths are both generated off the l-cam file i gave you set at 16 to 1 or 31.200 scale. air-poc1 after pocket path generation
was scaled back to 1.950 then you delete all layers except the pocket. then optimize, then i moved origin to center.you do origin the way you want. selected tool for the layer then posted code.this code works with mach3 X&Y scale set 1.000 .
air-poc2 was generated 31.200 and not scaled down. before loading into mach3 set scale X&Y to .0625 wich is 1 to 16 .when you check both files toolpath after loading you will see they are the same. this just shows differant ways to do the same thing.
keep in touch were all pulling for you.
bill
-
you aint dead yet, here is another pile of crap. heheheh!
The first thing i do after loading a file into l-cam is to turn leds off then turn the rapids off before doing anything. maybe that might be causing you a little snag.
keep in touch were all pulling for you.
bill
I am going to try to do what you described here. I never would have figured out this type of stuff. This is exactly what i need in the way of helping me and not doing it for me. I really appreciate your patiance and if i ever figure this stuff out, I will pay it forward for sure!!
-
Are you guy's sure your not screwing with the new guy! hhahahahh!
First of all i used the DOC's file to get the part ready to cut. Everything went perfect and was very easy to do.
I spent hours trying to replicate what was done and IM A FAILURE!! I cannot figure out what is different between the Doc's and mine. Here is what i tried. What did I miss? Is there something in the setup that i need to change? Why does it work on doc's computer and not mine?
Load AirCleaner4Test.DXF
Turn Rapids off
Turn Leads off
Move Chain#0 to new layer #3
Move Chain#2 to new layer #4
Move Chain#4 to layer#4
Move Chain#1 to new layer#5
Select layer#5
Click pocket tab
Click spiral, ccw, in-out, left
Click tool, 1/4, step 40, finish .048
Click create islands
click create pocket
Failure
Move layer #5 under layer Visible
click chain#11
click pocket
Failure
-
Hi Steve
here is a pic of my loading setup. this pretty much gets most of my stuff.
this is going to be a step by step of what i did to your dxf to make that l-cam file.
1.import file
2.turn off leads
3.turn off rapids
4.scale to check for X dimension , i wright down 1.950,close scale,make sure origin stays lower left
5.leave large outside chain in original layer,move second largest oval chain to next new layer
6.move big curly chain to next new layer
7.move top small chain to next new layer
8.move bottom small chain to same layer as top small chain
9.open scale and set X to 31.200 wich is 16 to 1
10.after scaling highlight each layer to make sure they are still where you put them
11.open scale again and make sure it set to 31.200, if it did not repeat steps 9,10,11
12.hit optomize once
13.highlight each chain and move lead arrows to middle of the flatest and longest line
14.check each chain and make sure your leads did not move
15.hit optomize again
16.save as your master l-cam
17.close l-cam
18.restart l-cam and load you l-cam file turn off leads and rapids. you should be ready to go.
bill
-
Just a comment Steve,
I guess it all depends on how you want to use LC and how you work. You can do all that doctf has shown, but,
for a newbie it is just not the way to go about it in my opinion. LC is a dxf importer and produces gcode based on the machining operations you want to do. LC is not a CAD program ( this is noted over 10 times in the manual).
Folks need to understand, that they need to think about all the different machining operations that will be done.
Then you can focus on defining cutting parameters to those different machining operations. Otherwise you may spend "hours" trying to manipulate chains or entities, tricking LC, or whatever, and even then, when it comes time to post you may not be able to get the operation's in the order you want to do them. Even selection of them can become a bear because of naming. Take a hard look at the manual.
Your air cleaner took around 35 minutes to draw and i was able to do all maching operations required for the piece.
This included redundant machine operations IE; after the horizontal lines where machined i would probably need to due another profile cut to remove some machining marks left by the cutter to clean things up. Very easily done by just adjusting cut depth by a few thou's.
In the end, you will have more success at getting the particular pathing more quickly, and not trying to do layout with LC which it really is not meant to
Have fun.... just a suggestion,
RICH
-
A few other comments,
I also leave the lead's and rapids turned off. LC will default all rapids to a z clear plane of 1 unit.
Lead's are added as required when appropriate. The rapids only make the viewing difficult.
I will usualy look at the rapids prior to posting the code to see that they are acceptable ( which will be the case
the majority of times ). And also always look for a rapid move that mmay cut thru the materail because of an X/y/z combination move as LC will sometimes do this and you need to modify the code so z is first before moving in the X or Y. When you change the machining order the rapids are changed.
RICH
-
LC is a dxf importer and produces gcode based on the machining operations you want to do. LC is not a CAD program ( this is noted over 10 times in the manual).
Hello RICH
I'm not sure what you think i did or am trying to do but i can offer this.
The part was drawn in Alibre V11. A drawing of the part was made and then it was exported as a Autocad V14 file as a DXF. I'm not trying to modify the part in any way, i just want to cut the part out as drawn.
-
Ok, so split the drawing into machining operations by putting them on associated layers like i did with the dxf
i posted. then all should be very easy and quick as all you need to do is define the cutting parameters to the correct layer.
RICH
-
LC is a dxf importer and produces gcode based on the machining operations you want to do. LC is not a CAD program ( this is noted over 10 times in the manual).
Hello RICH
I'm not sure what you think i did or am trying to do but i can offer this.
The part was drawn in Alibre V11. A drawing of the part was made and then it was exported as a Autocad V14 file as a DXF. I'm not trying to modify the part in any way, i just want to cut the part out as drawn.
Steve,
If you have the option of saving in AutoCAD 11/12 ASCII dxfformat, try that instead of Autocad V14, as that "mostly" worked for me with LCam.
Dave
-
steve
what budman said is good . v12 basically used here. my example was how i managed your drawing. l-cam does not like arcs on small parts. try drawing on many layers and scaled up, this helps.
avoid using offsets on pockets if you can, it might generate oversize code. l-cam has a lot of power ,but it does goofy stuff. when you draw big to go small it helps alot. it saves on crop circles too.
lately i have got in the habit of big drawing and using the scale feature of mach3 wich works really good.
bill
-
V14 is as far back as Alibre will let me go for DXF.
-
I would like to thank all those who helped. I have decided that manual milling is the way for me. For whatever reason my hardware/software wont do what yours will. I give up!
You guy's are awesome for hanging in there with me!!
Steve
-
steve
maybe your l-cam install was a bad one. do a uninstall and download a fresh copy of 3.00.2
your close, dont worry about the mule just keep on driving.
bill
-
I had a problem about a few weeks ago and tried that. It did'nt help solve the problem.
-
I think you fellows are missing the point Steve is trying to make(;-) LCAM "should" have been able to do the simple pocketing required WITHOUT having to resort to MAGIC MONKEY dust to get it to work. THere is NOTHING complicated in his drawing that I saw. He was NOT trying to redraw the part in Lcam just do the simple pocketing.
Steve just for the record I can't get it to work here either(;-) at your scale.
Large arc small arc an arc is an arc. The math involved is all the same. (;-)
THese are just some of the problems that PLAGUE newbees trying to use LCAM so they can "USE" MACH.
(;-) TP
(;-0 TP
-
Steve just for the record I can't get it to work here either(;-) at your scale.
For the record, I cant get it to work at any scale. I have worked with it at 4X, 10X, 16X, and it simply will not pocket the center of the inner oval and leave the ribs as islands. Using Doc's file it will do everything that I wanted.
Hey Doc, did you use my dxf (v14) file or did you convert mine to another version of dxf (V12) before working with it? There has to be a reason it works everywhere but here.
-
steve
i used your file. the step by step is exactly how i did it.did not move any chains or alter them. it went real easy.
maybe it might be a graphic card thing. uninstall your card,shut down computer cold,let it reinstal the card. check for a driver update.
like you say it might be something else. do you have another computer you can try.
vmax there is a lot of things wrong with l-cam and the math is a big part of it. art said when he gets lathe done he is going to clean l-cam up and merge them.
l-cam does run better on more modern computers with better graphics cards. but that does not fix the program.
bill
-
steve
i used your file. the step by step is exactly how i did it.did not move any chains or alter them. it went real easy.
maybe it might be a graphic card thing. uninstall your card,shut down computer cold,let it reinstal the card. check for a driver update.
like you say it might be something else. do you have another computer you can try.
vmax there is a lot of things wrong with l-cam and the math is a big part of it. art said when he gets lathe done he is going to clean l-cam up and merge them.
l-cam does run better on more modern computers with better graphics cards. but that does not fix the program.
bill
I can try the computer in the garage that actually runs the mill. Lcam is installed out there. I'll try it right now!
-
steve and vmax
i forgot to mention that if you have trouble with a dxf ,post it up here with a description and the tool. we will try to get you a good l-am file back that you can use.
everybody is in the same boat with l-cam until the rewrite.
bill
-
HECK right now I can't even download a fresh copy of the DXF. Windows refuses to recongnise the DXF extension on the download.
Time to call it a day I think, (;-) TP
-
Vmax: I tried the garage computer and got the same result.
Doc: You provided a file thats works perfect. I could cut the part right now. It has become more about learning something rather than making something.
I'm done for the night myself!!
Steve
-
good night guys we will play tomorrow. steve i will download this new dxf and look at it.
bill
-
Hi Steve,
Don't know why your going thru a lot of trouble for nothing. Let me make my point then i will go to
the sideline. In the picture on the left the red lines are actual paths of a ball end mill. If spaced appropriately you
will get the scalloped affect shown in the midle of the picture. On the right is your drawing and i
have just added the red lines which indicate the tool paths. If the psacing was right you would get
the affect you are after with no problems creating the code and screwing around with offsets or
pockets as all you need to do is defined the cut paramaters.
All of that would be one chain if you put it on one level of the drawing.
Now i would first machine the "blue lines" because this way the tool need not constantly plunge into
the material.
Then machine the paths.
Then re-machine the blue lines again to get rid of any plunge marks.
The pink dots would probably be done with a square end mill and not a ball end.
The light blue dots are all done as a drilling.
Just some thoughts on it all,
RICH
-
steve
downloaded that last dxf you put up. it was a real pain. you got a right to go nuts over this. this one had more trouble with archs than the first. i made you a l-cam for this one.
i think this method might help you through this, plus show you another way to use l-cam. in this example we are going to use mach3 as a filter.
1.import file turn leads off
2.then scaled up 16 to 1 because the cutter you want to use is .015625
3.optomize
4.check scale
5.set origin
5.pick a tool,set all layers the same
6.post and save code
7.close then open l-cam
8.import back into l-cam from mach3
9.now you have a file to save as a l-cam file
the l-cam file i gave you was generated this way
bill
-
Hi,Rich
steve has an idea of what he wants to do. he is just having a real hard time of getting his cad to work with l-cam. his last dxf worked worse than his first.
he cant save in v12 so it makes it a little tougher but his dxf can work. you keep pushing ideas on him and dont let up we got to get him trained or totaly confused. haha!
you cant quit now you are in as deep as i am.
bill
-
HMM.....
For training, do each of the tutorials in the manual. For confusion just ask me. ???
Not all DXF's are created equaly, maybe, Apsire should be added to my list!
RICH
-
HMM.....
For training, do each of the tutorials in the manual. For confusion just ask me. ???
Not all DXF's are created equaly, maybe, Apsire should be added to my list!
RICH
Hi Rich!
I read the manual, every word, and did the tutorials that related to milling. I revisited the manual several times before i came to the forum for help. The problem is'nt that i don't know what to tell LC to do, it's LC wont do what i tell it.
There is an obvious problem with my dxf files as even the seasoned vets are having big problems. Like i said many times, I used Docs Lcam file and everything worked exactly like i wanted it to.
For me, this isn't about getting a file that works, I have one. This is about finding a way for me to get from Alibre to Mach3 without having to rely on you good people to generate files for me. If i have to import into lcam, then save and open mach3, then import to lcam again, thats what i'll do if it works.
I just need to find a way to get there.
-
steve
downloaded that last dxf you put up. it was a real pain. you got a right to go nuts over this. this one had more trouble with archs than the first.
I had one dxf that made the part look like a football with a big bulge in it. That dxf is no longer with us.
-
if spacing was right you would get the affect you are after with no problems creating the code and screwing around with offsets or pockets as all you need to do is defined the cut paramaters. All of that would be one chain if you put it on one level of the drawing.
You have to remember im new at this. Are you saying I can define my own tool path somehow without using the pocket and offset tabs?
Now i would first machine the "blue lines" because this way the tool need not constantly plunge into the material.
How would i go about doing that. Would i click on those entities and create a tool path next to those?
I'm willing to learn anything you are willing to show me. Take that dxf file and describe how you would do things in Lcam as Doc has. I'll try to replicate it step by step and learn something new!!
Thanks Rich
-
Steve,
How about this, since you can not save in the AutoCAD 11/12 ASCII dxf version, how about trying a free CAD program that will. You can still create your drawing in Alibre but after you've saved your file to dxf, open it up in ProgeCAD, and then just save it as a AutoCAD 11/12 ASCII dxf, and see if that helps you. The worst that can happen is it doesn't work and you just uninstall the CAD program :)
Don't let the fact that this program scare you because it's free. It's a very powerful program and in most cases, it has way better luck opening all kinds of dxf types that the "real" AutoCAD won't.
The download link is at the bottom of the page under: DOWNLOAD progeCAD 2008 Smart!
http://www.progesoft.com/en/smart-2008
Hope this helps out.
Dave
-
Hi Steve,
This is what I do to machine right ON a line as RICH mentioned.
I define a tool as "ON VECTOR" - Diameter 0.0001
Select this tool and do an offset.
Use whatever *actual* tool you wish, just keep in mind that the cut will be out from the drawing .00005 ::)
Close enough for me ! :)
Most likely a better way tho.
Russ
-
...or, dont select any of the tabs. code will be generated on any line using the info for that layer.
-
Steve,
DXF IMPORTING - I was able to import your dxf files into CAD, but, there can be problems with DXF
files. Here is the problem, kind of, the way i understand it. As programs have matured, say 3d was added and thus, the dxf file content also changed to suite to contain that additional info.Version 12
DXF dosn't contain all or a lot of info and represents data differently. ( i have a write up on dxf files in
the LazyTurn manual as an appendix. SO the info from the providing program can't be read correctly
by the recieving program during the import. You will find that if you try to import your dxf files by an
old program that it may or will bomb. Newer programs will import it but you'll get error messages.
So LC's importer is lacking and the newer creating program has some undesirable things in it also.
But what is a person to do if his dxf don't import, well............i don't have a simple answer!
As a suggestion you may want to try some free CAD programs and see if they will import and
export your files appropriately for use. You may want to ask Alibre what they recomend. Changing
the dxf file exporting is a book in itself and frankly even advanced folks can have trouble, if there are
even ways to change the exporting.
------------------------------
"Are you saying I can define my own tool path somehow without using the pocket and offset tabs?"
Exactly. You can just draw lines, arcs, or whatever in your CAD drawing and then define the cut
parameters for them, your basicaly doing the pathing and LC is just writing the Gode for them.
I think the only place i talked about this in the manual was in the lathe tutorial "EXTRA LINES".
This can come in handy since sometimes, for what ever reason ( including some high end
programs) you just can't get an area to pocket. It's 99% and what do you do for that 1%, easier to
draw a few lines then spend hours fooling with the program! The higher end programs provide you
CAD, and if something bombs on inport, well they send you over to the cad sections so you pick
and choose what you want to do. That is what i did in my drawings for the air cleaner. It is easier to
just draw the paths and have LC generate the code for them. LC generates code for only the stuff
that is "enabled" allowing you to pick and choose machining operations.
-----------------------------------
"How would i go about doing that. Would i click on those entities and create a tool path next to
those?" YES
Think in terms of machining steps. How will this piece be machined? In what order? And then
create your drawing appropriately by having those entities / chains / pathing on their own layers.
You will know each via the project information at a glance.
For example:
1.Using a .016" cutter you would have a chain for the inside boarder on it's owne layer, select only that layer, turn off / unenable all the other layers, define the cut paramters for that layer ( would be based on the tool you will use for that machining operation ( say machine down to a .016"
depth). Post code and machine it.
The air cleaner has a inside boader. So if you use a .016" dia ball mill the offset would be .008".
Well you can create an offset for it in LC...or ....heck in cad do the pathing for it and it's already on
its onwe layer. You don't want to do this in general, but, for some stuff it may be easier, at times.
2. Now you would machine all the paths that make up the "ribs"/ scalloped areas, Each of those
cuts, start and end in the inside boarder. That will leave little dots from the ball mill and you may
not want to see them from an asthetic point of view.
3. After seeing how 1 & 2 actualy machined, you may want to remachine the inside boarder but this
time increase the cut depth by a smalll amount. say .018 which wil remove the marks and look
clean.
So you have a layer which represents a machining step, you simple tell LC the cut paramters for
that step, post and machine.
RICH
-
I tried that myself, His dxf to Progecad to V12 dxf. Still did not work. Next IF I can get it downloaded to the shop puter I wil do it in Acad directly. I can scale it up and down to no avail. NOTTA
I can get it to do a pocket BUT it is the entire area, it does not SEE the fins. OR it just ignors it all and does nothing. I could be the puter and Lcam It is running on vista at the house.
(;-) TP
-
The file imports into AutoCAd ver 2000 and up, bombs in old microstation versions, is ok in the newer microstation versions like V8.
RICH
-
I tried that myself, His dxf to Progecad to V12 dxf. Still did not work. Next IF I can get it downloaded to the shop puter I wil do it in Acad directly. I can scale it up and down to no avail. NOTTA
I can get it to do a pocket BUT it is the entire area, it does not SEE the fins. OR it just ignors it all and does nothing. I could be the puter and Lcam It is running on vista at the house.
(;-) TP
At least i know it's not just me.
Hat's off to Doc! What ever voodoo you do, it works!!
-
So Rich, what you are saying is to draw the tool path in cad instead of the part. Then tell Lcad to cut on the line.
Interesting approach!
-
Steve,
Now you got it. ;)
You need to do a layout, just add the pathing ( because its easy ), and in this case / your project, it's actualy eaisier and you get exactly what you want without fidling around trying to get LC ( or some other CAM program ) to generate the pathing. DO NOT RELAYER as LC will redo all your layering based on what it thinks the machining order / optimal pathing should be.
LC is just an importer! When you try and use offsets or whatever you are just tricking the program to get what you could have just drawn in CAD. Not the norm but very effective in use.
RICH
-
good morning steve
ok here is what i got,there are two forces working here and they are both bad. the first we know l-cam dont like small archs that it did not generate. the second is that your cad as nice as it draws has bad blood running in its veins that
l-cam can see but we cant. so when you try to do something with the original dxf l-cam is trying to work with the bad blood. everything come out sick. so what you have to do is filter the blood. believe it or not mach3 and l-cam makes
a good filter. your cad does draw nice as compared to others. so here is the plan to filter the blood. attached are two taps that i filtered, and they are g-code clones of your dxf.
the move is to take you dxf and just convert it to g-code, load it into mach3 then import back into l-cam. that filters the bad blood. you can play with it at the original scale and see how much better it works with l-cam. but you will still
have trouble with pockets at that size, so scale up to pocket. this should help you smooth out the proccess.
bill
-
:) See, this is why I try to keep from helping as you guys are just awesome/amazing and I think I only make things worse by getting involved. :D
Dave
-
Bill,
Good thought but ........
Carefull on the "backploting" into LC. If the file is generated from LC and posted into Mach and then returned to LC it may go well. If a file is not originated from LC, you open a Gcode file in Mach and the bring back into LC things can get very screwy. Certainly worth the try.
Page 14 of the manual, "Load current Mach3 File" definition / remark.
Just a comment so folks don't think you can backplot with great success.
Bill, how about an older version of like Mach2 which inported DXF's? Don't have one installed but may be a free
fix. Worth a try!
Dave........we all have an open mind here, so if you think of something ,post.
RICH
-
Hi,Rich
what you are saying about the mach3 import is true. the thing about the backplot move is to try to strip the dxf down to only the chains that are to be used. the target is to get a clean g-code drawing.
when you import it back in l-cam is going to move the chains as it sees fit, but it does not hurt the chains. you then move all the chains to new layers and arrange the layers to what you want. delete all old
layers. scale it up , do an optomize, then save as a l-cam file. now you have a master l-cam. another thing i do that helps alot is to draw a box border around the part wich will give l-cam 4 points for maximum
extents to locate of off while you work on the project. then you delete it like everything else before posting.
bill
-
Rich
here is some lay work that i have been working on. these letters are .1875 tall. everything is done with mach3,l-cam and the text editor in mach3. the fonts were TT imported into l-cam.
there was alot of scaling and backplotting to get the master l-cam, then it was smooth sailing from there. as crappy as l-cam is , i have alot of fun with it, plus it has a ton of power. all the lays
are done and this week i do the pockets. the code and the butt are ready .
bill
-
Hey Doc!
You are going to love this one. I opened the dxf into Lcam. Did all the move, optimize, post hocus pocus and looked in mach3 and there was the air cleaner. THE AIR CLEANER TOOL PATH WAS THERE!
I go back to Lcam and click the load current mach3 file button and guess what happens.. . . . . .
The image of a file that i havent worked with in 2 weeks is in the Lcam window!!
2 WEEKS!!
Got a fix for that one!! Haahahahhahhahhha!!!!
Gotta go bang my head on the garage wall!
BYE
-
After all the hoopla, here is the finished product. Try not to laugh, it's only my second attempt at Gcode.
-
steve
you had that all along and were just messin with us. now quit clowning around and get to work.
bill