Solidcam and solidworks settings

[Raf-1200]

Struggling with a couple of things as a beginner. Been making parts for a while but I've managed to circumnavigate but it's time to sort it out lol.

When I start every milling process the z axis moves up. If I am using a fixture to hold my piece it will normally move up too far. I think about 100mm. Goes to the correct spot, rises up and comes back down to start the cuts. How do I make this not happen or change the height that it does happen? Thought clearance levels but now I know that's incorrect.

Second thing is when the job is finished the mill head moves to a position far from the job. Would be great to just have it stop at clearance height etc...
Currently I have a 900 x 600 and am using ncstudio. When I Choose a machine in solidcam I pick the gMilling_3x. Don't ask me why. Tried it a couple of years ago and it worked

Any help would be appreciated.


Mostyn Cafe & Customs
Builds and Parts
www.mostynindustries.com.au

Similar Threads:

• Need Help!- Solidworks, to solidcam, to mach 3.
• Need Help!- SolidWorks 2010 and SolidCam
• Solidworks SolidCam help
• Need Help!- Solidworks 2007 and SolidCAM
• SolidCAM & Solidworks vs. MasterCAM

[Txin]

These two questions means Some Setting parameters in the Coordinate System of SolidCAM do not go right, Suggest you to change the parameters about the clearance in the windows of the Coordinate System.

if you need any help about solidcam(post or others), please contact me by email, solidcamtx@gmail.com.

hope it can helps you.

[Raf-1200]

Hey txin... That's what I thought to.. Mucked around with clearance and it helped but I still have the issue with the heading shooting off when it finishes to some unknown location... Ncstudio or solidworks issue?

[Rick_B]

Raf-1200, is your machine going to home zero when it finishes cutting? I was using gMilling_3x on my Fanuc controller and It did that after the final.

Rick

[Raf-1200]

I believe it is Rick. So what to do about it?

[Rick_B]

The little bit I know about this, it's a line in the post-processor which sends the machine to home. I was told it's a safety/convenience thing. I know my machine does it before every tool change, but I had my post written so that after the finish it still parks the head at zero, but it puts the bed center of the doors and close the the front of the machine.

Rick

[T D]

Z issue
Open your CoordSys Data. Check the tool start level (Between operations, Z will go to the clearance after the cut then to the tool start level then back to clearance then safety distance then to cut level.) I would think you want the tool and clearance level the same. The tool start level is used to turn on any coolant, air blast or miscellaneous options. Unfortunately the gMilling_3x post processor I use does not use the tool start level, but HASS-3x does use the tool start level.

X Y Z Homing.

Sounds to me like you need to get to know G28, G53, G90, and G91.

stock output
N152 G00 G28 G91 Z0
N154 G00 G28 G91 X0
N156 G00 G28 G91 Y0

What I think you want.
N152 G00 G28 G91 Z0
N154 G00 G28 G90 X12.0
N156 G00 G28 G90 Y12.0
(the Z would go to it's 0, X would move 12.0 inches in the + direction then the Y will move 12.0 inches in the + direction.)

Save time and move the X and Y together. Use caution this is a diagonal move in X and Y
N152 G00 G28 G91 Z0
N154 G00 G28 G91 X0, Y0

Use G53 to bring a table style mill to where you need it at the end of it's run. I use this on a Haas VM3. CAUTION G53 IS NOT A MODAL COMMAND.

N152 G00 G28 G91 Z0
N156 G00 G28 G91 Y0
N154 G00 G53 G90 X20.

The above lines will bring Z and Y to their 0.0 then move my 40 inch table to it's center for easy unloading.
Hope this helps.

[radboi22]

I believe it is Rick. So what to do about it?

I had this problem when I first started. I used gibbscam first, and I had the issue of the machine trying to run off and crashing. I figured out that in mach 3 I had to set the Machine Coords, because the code tells mach3 to go to machine cords rather than work cords.