new user confusion...

[Spinnetti]

I imported a dxf and set some tool paths, but in the resulting gcode, it wants to move 7" away from the part. I assume its because the origin is in the wrong place. How do I move it?

Also, not sure yet, but it looks like the part got scaled way up somehow. How do I make sure its 1:1?

Thanks.

[chuy]

Translate/all/entities/between points/ it will ask point to translate from,I usually pick the point I want as my origin...click that point....it will ask translate to...I usually say origin..
and done... The other part analyze the drawing...analyze/between points...I'm assuming you know how big it shuld be..click on a couple of points and see if there is a difference...let's say you distance between your points should be 7" and now it's 14 if that's the case than go transform/scale all entities from origin and scale the difference...if its twice the size than your scale factor is.5

Hope that helped

[Spinnetti]

Originally Posted by chuy Translate/all/entities/between points/ it will ask point to translate from,I usually pick the point I want as my origin...click that point....it will ask translate to...I usually say origin.. and done... The other part analyze the drawing...analyze/between points...I'm assuming you know how big it shuld be..click on a couple of points and see if there is a difference...let's say you distance between your points should be 7" and now it's 14 if that's the case than go transform/scale all entities from origin and scale the difference...if its twice the size than your scale factor is.5 Hope that helped

Thanks. I figured out the scaling thing.. it was how Solidworks was exporting.. fixed that. I'll try moving the part again. I got it to drag ok, but not so it would be on the origin.. didn't see that - will look again.

Last issue is hard to describe. I'm cutting what essentially is an open pocket, but in the middle of the stock.. not sure how to get it to lead into the material. I keep getting some kind of errors unless I do it as a countour (contrary to the image, much of the open area is cut just 1/2 way through), but that leaves material in the middle (its the lower scissor link in the picture, where the big open area is in the middle of the stock - had to do it that way so I could cut the outside contour without dropping off the part)

[cadcam]

when picking the open detail in the pocket tool path. there is an option for open pocket. make sure this is set.

[Spinnetti]

Originally Posted by cadcam when picking the open detail in the pocket tool path. there is an option for open pocket. make sure this is set.

Thanks..
Yep, did that.. got errors. Tried to work around it, but instead busted a brand new carbide bit <grrr>. I forget what error it gave me, but I haven't figured it out yet. I hand edited the G-code, but still need the pocket function to clean up the middle of the cut. Here's an image of what it looks like in master cam. The innermost part is only .050 deep, and the outer part is all the way through. So far I did it as 3 contour cuts, but had to edit in the tool clears, ramps into the work etc to get it to work in gcode. I'm sure there's a way to do it, but I don't know it.

[cadcam]

Well this alwas help me help you give me that file I will adjust it and give it back.

[Spinnetti]

Originally Posted by cadcam Well this alwas help me help you give me that file I will adjust it and give it back.

Thanks for the help! I can also send a couple annotated pics of what I'm trying to do if that helps. Key thing is I need to cut as much as possible in one pass. Because the part is very small as well as tapered, It's not practical to do any secondary ops. The outer contour is ok, but I essentially need to do two open pockets for the inner contours, one .050 deep, the other through. Both the inner cuts need to ramp into the work due to not having a pilot hole and being in the middle of the stock (.5 wide, .125 thick, feet long, hanging out of the vise on the left side about 1.250). The last step is to cut the part off the base stock. I can also take a picture of the setup if that helps. I realize this is all probably pretty basic, but until I "get it" its kinda frustrating. Finally, do you know what option I should pick to post gcode for Mach3?

Thanks again!

[jolafson]

Here it is, take a look at all your toolpath parameters, make sure i put the right depths, tools, absolute/incrementals etc... back in!

The big problem was overlapping entities. Two ways to fix these.

1.) click on the icon that looks like two puzzle pieces, one red and one blue. It will say "run user apps". This is your CHook folder. Double click on findoverlap.dll
select "all" entities, then press enter. If you have them (theree were 26 on that file), it will pop up a box on the screen, just press cleanup, and it will tell you how many it found.

2.) select all your lines, making sure to click on them only once. Then, translate them to a different layer, and use that layer to toolpath them on.

The first way works 99% of the time, so that's what i'd use. Overlaps make it impossible to chain properly, because the program doesn't know whick line you're wanting to chain to. Clean single lines of geometry are waht MC loves, as does any programmer.

It took me a while to learn that trick, then i finally "got it".

Hope this helps you"get it"

Keep the greasy side down, and the pointy end forward, and it'll all be ok!

[Spinnetti]

Originally Posted by jolafson Here it is, take a look at all your toolpath parameters, make sure i put the right depths, tools, absolute/incrementals etc... back in! The big problem was overlapping entities. Two ways to fix these. 1.) click on the icon that looks like two puzzle pieces, one red and one blue. It will say "run user apps". This is your CHook folder. Double click on findoverlap.dll select "all" entities, then press enter. If you have them (theree were 26 on that file), it will pop up a box on the screen, just press cleanup, and it will tell you how many it found. 2.) select all your lines, making sure to click on them only once. Then, translate them to a different layer, and use that layer to toolpath them on. The first way works 99% of the time, so that's what i'd use. Overlaps make it impossible to chain properly, because the program doesn't know whick line you're wanting to chain to. Clean single lines of geometry are waht MC loves, as does any programmer. It took me a while to learn that trick, then i finally "got it". Hope this helps you"get it" Keep the greasy side down, and the pointy end forward, and it'll all be ok!

Thanks - I'd never have figured that out!
Actually going to an R/C event right now, but when I get back I'll try it and report back. Thanks again

[CAMCRASH]

Spinnetti,

Just as a note for the future.
If your part was not drawn at the same origin that will be used for machining
There are 2 way you can adjust this without moving your part

OPTION 1 --
1) click the WCS in the lower right hand of the MC screen
select view manager
2)In the main screen set the WCS, tool plane & construction plane all to the same view you plan to machine in ( front / top / bottom / etc )
The = icon will move all three in one step
3)a) Click on the pointer icon ( moves you to main MC window )
Select a point / intersection you would like to call zero.
3)b) If you want to select or move a individual axis
Right click in the axis of choice and select option from drop down &
select new feature

This moves the Zero point for all machining operations on that selected plane to the one you just set

OPTION 2 --
1) Select tool path type & tool path geometry
2) In tool path manager click on the planes button
( bottom center of window)
3) Click double right hand arrows ( Lower Left in window )
4) Select Plane by using plane selection button in first box
( plane selection button is left of the pointer button )
5) Set part origin as seen in OPTION 1 step 3a / 3b

NOTE: IF YOU ARE USING A ROTARY AXIS THE WCS WILL NEED TO BE SET TO
THE PLANE OF THE AXIS ROTATION IN THE WORLD COORDINATE VIEW
AND THE TP AND CP WILL NEED TO BE SET TO THE PLANE THE THAT
THE WORK WILL BE COMPLETED ON ( ONCE AGAIN ) WORLD COORDINATE VIEW.

[Spinnetti]

Originally Posted by CAMCRASH Spinnetti, Just as a note for the future. If your part was not drawn at the same origin that will be used for machining There are 2 way you can adjust this without moving your part OPTION 1 -- 1) click the WCS in the lower right hand of the MC screen select view manager 2)In the main screen set the WCS, tool plane & construction plane all to the same view you plan to machine in ( front / top / bottom / etc ) The = icon will move all three in one step 3)a) Click on the pointer icon ( moves you to main MC window ) Select a point / intersection you would like to call zero. 3)b) If you want to select or move a individual axis Right click in the axis of choice and select option from drop down & select new feature This moves the Zero point for all machining operations on that selected plane to the one you just set OPTION 2 -- 1) Select tool path type & tool path geometry 2) In tool path manager click on the planes button ( bottom center of window) 3) Click double right hand arrows ( Lower Left in window ) 4) Select Plane by using plane selection button in first box ( plane selection button is left of the pointer button ) 5) Set part origin as seen in OPTION 1 step 3a / 3b NOTE: IF YOU ARE USING A ROTARY AXIS THE WCS WILL NEED TO BE SET TO THE PLANE OF THE AXIS ROTATION IN THE WORLD COORDINATE VIEW AND THE TP AND CP WILL NEED TO BE SET TO THE PLANE THE THAT THE WORK WILL BE COMPLETED ON ( ONCE AGAIN ) WORLD COORDINATE VIEW.

Thanks for that tip.. I was trying various methods to fix that, and it was kinda messy. One other thing thats still not happening is ramping into the cut where it goes in the middle of the stock - I'll try tweaking that again today to see if I can get it to do it (I don't want to plunge in for fear of breaking my cutter)

[CAMCRASH]

I have not seen a way that you can ramp from a entry point / origin
If you need to use a ramp, from what I have seen is that is picks a
start point based on the data you give it

I perfer to use the helical
With this you can specify some additional data and control points
Try This
1) When selecting geometry
a) Select Start Point ( Use Point Icon in chain manager )
b) Select Geometry / Pocket Chain ( Use Chain Icon )
c) Select The Initial Point ( Use Point Icon )

This will tell MasterCam to do this
Start at a specific point
Run Chain
Return To Initial point for next depth of cut

This works in both pocket & profile paths
In LeadIn/LeadOut On profiles you may need to select use entry/exit point check boxes ( There is on box for entry & one for exit )
You shouldnt need to do this on pocket

Now insted of using a ramp
2) Select pocket style to any but zig/zag
3) Click entry Helix/Ramp button
4) Click on the Helix tab
5) Set parameters & Click the Center On Entry Point Check Box
This forces The tool-path to do a helical entry around that point