Hey Guys,

Thanks for all the help thus far, it is finally starting to click a bit. I manage to work out the last part I posted. I have another part that is giving me problems. It will be machine on two sides, right now I am trying to get the top set up. I first started my making a profile cut around the out side perimiter and it worked fine in SolidCAM.
Next I try to cut out the slots. I first tried using a profile but there as no complete chain to do this. Then I tried using a pocket but could not get it to work.
Then I tried a slot, which now I think is the best method but I could not figure it out. Can anyone offer some suggestions as to what operation I should be using? Please let me know if you have any questions. Here is my part file and some pics. May be someone can set up that part in SC and send it to me so I can see how it was done?

Thanks,
Skipper

Hi Skipper
I looked at your drawing.
The slot sketch is not fully defined. This could be causing you problems.
You should be using fully defined drawings if you do not want surprises.
I also notice that the drawing dimensions in decmal inches.
As your slot is in 16th I suggest you change your dimensions to the nearest 64th of an inch. It should save conversions.

I do not have time to do it but I think you should be using the slot tool if you have a 7/16th tool. it could work with a left and right slot using a 1/4 in tool.

Also a 1/in tool in profile will cut the slots.

If you do not get it email me.

Doug

Hi Skipper
I finally got some time.
Your 7/16th groove is 11mm wide so if I use a 6mm(1/4inch) end mill I will cut a pocket 11mm wide.

So cut a profile cut around the outside as you did.
I then cut a profiles around all the raised portions and got the required grooves.

Finally I cut a slot with the 6mm (1/4inch) cutter.

One trick used was to turn the peice over so I could mark the slot.
Attached is your revised drawings and my tool paths.
If was going to cut the path I would move the start points on the second path, but who cares the mill will cut it quicker than I can correct it.

Doug

Hey Guys,

Thanks for all the help thus far, it is finally starting to click a bit. I manage to work out the last part I posted. I have another part that is giving me problems. It will be machine on two sides, right now I am trying to get the top set up. I first started my making a profile cut around the out side perimiter and it worked fine in SolidCAM.
Next I try to cut out the slots. I first tried using a profile but there as no complete chain to do this. Then I tried using a pocket but could not get it to work.
Then I tried a slot, which now I think is the best method but I could not figure it out. Can anyone offer some suggestions as to what operation I should be using? Please let me know if you have any questions. Here is my part file and some pics. May be someone can set up that part in SC and send it to me so I can see how it was done?

Thanks,
Skipper

If you want to machine a profile for which edges don't exist on the part, do this.

Go to the SolidWorks Feature Tree

Right-click on "CAM" and then click "Edit Part"

Pick a plane (or a flat face) parallel with the geometry you which to profile and insert a sketch.

Use SolidWorks tools such Convert Entities or Intersection Curve to transfer the geometry you want to the sketch. Then draw in the bits that are missing.

Exit the sketch

Go back to SolidCAM and when you define the SolidCAM profile geometry, pick the sketch lines. Violá. (There is a faster way of selecting the sketch using the "CAD Selection" button)


I do this sort of thing a lot to create working area boundaries etc.

Thanks Bob
I did not know I could do that. At least three locals will find it a big help.

Doug

If you want to machine a profile for which edges don't exist on the part, do this.

Go to the SolidWorks Feature Tree

Right-click on "CAM" and then click "Edit Part"

Pick a plane (or a flat face) parallel with the geometry you which to profile and insert a sketch.

Use SolidWorks tools such Convert Entities or Intersection Curve to transfer the geometry you want to the sketch. Then draw in the bits that are missing.

Exit the sketch

Go back to SolidCAM and when you define the SolidCAM profile geometry, pick the sketch lines. Violá. (There is a faster way of selecting the sketch using the "CAD Selection" button)


I do this sort of thing a lot to create working area boundaries etc.

Hey Guys,

I still have some problems. I fixed the model a bit, I did not actually give the top slots dimensions so I gave them .5" width and .1 depth.
Doug, I tried using a profile like you suggest but it is not a complete profile outline from on top. I think that if the radius on each of the slots were not there then it would be easy to use a profile of slot. I think I need to do what bob is suggesting but I could not figure it out how to make the chain profile.
I also tried using the slot command again but when I chose the "point to point" command the start of the slot line kept starting at the solidworks part coordinate center. It would not allow me to grab the mid point of both end of the slot.

Thanks,
skipper

I have tried Bob's solution and it works great'

When you use the profile you are cutting out the top, The slot is formed because the cutter is over half the width of the slot. So when you consider what you are profiling is the top. So select the tops one by one with the constant z option. When finished you will have series of islands and will cut the out side profile in places. Look at the solid not the goal. The corner fillets are no problem. Remember that you must select the lines in order and you may have to zoom in on the corners and then out again.

To cut the slots turn the model over and select the edges on constant Z. Turn the model right way up and proceceed as normal. I cut the slot with a the same cutter as I used for the groove.

I attached the drawing to my posting but it did not upload. If you still have problems I will send them directly to you.

Doug


Hey Guys,

I still have some problems. I fixed the model a bit, I did not actually give the top slots dimensions so I gave them .5" width and .1 depth.
Doug, I tried using a profile like you suggest but it is not a complete profile outline from on top. I think that if the radius on each of the slots were not there then it would be easy to use a profile of slot. I think I need to do what bob is suggesting but I could not figure it out how to make the chain profile.
I also tried using the slot command again but when I chose the "point to point" command the start of the slot line kept starting at the solidworks part coordinate center. It would not allow me to grab the mid point of both end of the slot.

Thanks,
skipper

Thanks Bob
I did not know I could do that. At least three locals will find it a big help.

Doug

You don't even have to "edit cam part", just click on a face and the SolidWorks pop-up will let you create a sketch right there. Like Bob, I seem to do this a lot.

I've noticed that the Constant Z HSM operation is pretty lame for profiling. You have to turn the accuracy waaaaay up and you still get jerky toolpaths. On parts with straight sides I get a much better surface finish by creating a sketch of the profile and then using it to drive a profile operation.

Joe

You don't even have to "edit cam part", just click on a face and the SolidWorks pop-up will let you create a sketch right there. Like Bob, I seem to do this a lot.

Thats right, SolidWorks puts the sketches in the Assembly. However, if you have big complex parts with lots of sketches for profiles, work areas etc. then putting sketches in the Assembly really slows things down as the Assembly keeps rebuilding. If you put the sketches in the CAM part, things are much faster to load, save and edit (but only for complex parts).

Another trick I have is to create a profile using edges and point-to-point in SolidCAM, saving the job, then little expand box next to the job in the Job Tree. This shows the geometries used - right click the geometry and select "Generate Sketch" which creates a sketch in the CAM part perpendicular to the Z axis for that job (I do a lot of 5 axis stuff and it is not unusual for me to have 20+ work co-ordinate systems). Then you can edit the sketch to give exactly the profile you need. Finally, right click the geometry again in the Job Tree and select "Edit" and choose your sketch. I fin thie really useful for those awkward little corners where you have defined the Co-ordinate System using the "Normal to Current View" option to get tool clearance.