I want to skim off (0.020") along the edge of a square runner on a plate.
Automatic Feature Recog finds the geometry in the model where I chamfered the edges by .020 just fine.
However when I simulate running a chamfer or ballnose mill, the operations menu is blank in the depth column for the seven operations I need.
Any suggestions about how I might get this operation to engage the work?
Thanks!
Bruce
--------------------------------------------
Hello @Anonymous,
Welcome to Autodesk Community!
The supplied image clears that you wish to have depth of a 3D surface milling feature within the Operation list.
At present we cannot get the depth value of surface milling feature within the Operation list.
Also, I would like to inform you that this has already been raised to the FeatureCAM Development Team as a feature request.
Thank You.
Robert,
Thank you for your kind response.
The depth column being missing might only be a symptom of the problem as the simulation skips the last seven operations and the times for each are small or zero. (OP 12 through 18)
Op: 11 side3 (finish), Fixture 1
F/S: 5200 RPM, 17.7 IPM (0.0009 IPT)
Tool: #3 (0.1875 4 Flute Carbide TiAlN, 0.1875 in.)
Depth: 0.1000 in.
Other: Stepover: 0.0234 in.
Time: 3:25.9
Est. HP: 0.06
Op: 12 srf_mill1 (finish1, z level), Fixture 1
F/S: 5200 RPM, 8.9 IPM (0.0009 IPT)
Tool: #4 (0.1875 2 Flute Carbide TiAlN, 0.1875 in.)
Other: Stepover: Adaptive
Allowance: 0.0000 in., Tolerance: 0.0010 in.
Time: 0:11.8
Op: 13 srf_mill2 (finish1, z level), Fixture 1
F/S: 5200 RPM, 8.9 IPM (0.0009 IPT)
Tool: #4 (0.1875 2 Flute Carbide TiAlN, 0.1875 in.)
Other: Stepover: Adaptive
Allowance: 0.0000 in., Tolerance: 0.0010 in.
Time: 0:00.0
Op: 14 srf_mill3 (finish1, z level), Fixture 1
F/S: 5200 RPM, 8.9 IPM (0.0009 IPT)
Tool: #4 (0.1875 2 Flute Carbide TiAlN, 0.1875 in.)
Other: Stepover: Adaptive
Allowance: 0.0000 in., Tolerance: 0.0010 in.
Time: 0:00.0
Op: 15 srf_mill4 (finish1, z level), Fixture 1
F/S: 5200 RPM, 8.9 IPM (0.0009 IPT)
Tool: #4 (0.1875 2 Flute Carbide TiAlN, 0.1875 in.)
Other: Stepover: Adaptive
Allowance: 0.0000 in., Tolerance: 0.0010 in.
Time: 0:00.0
Op: 16 srf_mill5 (finish1, z level), Fixture 1
F/S: 5200 RPM, 8.9 IPM (0.0009 IPT)
Tool: #4 (0.1875 2 Flute Carbide TiAlN, 0.1875 in.)
Other: Stepover: Adaptive
Allowance: 0.0000 in., Tolerance: 0.0010 in.
Time: 0:00.0
Op: 17 srf_mill6 (finish1, z level), Fixture 1
F/S: 5200 RPM, 8.9 IPM (0.0009 IPT)
Tool: #4 (0.1875 2 Flute Carbide TiAlN, 0.1875 in.)
Other: Stepover: Adaptive
Allowance: 0.0000 in., Tolerance: 0.0010 in.
Time: 0:00.0
Op: 18 srf_mill7 (finish1, z level), Fixture 1
F/S: 5200 RPM, 8.9 IPM (0.0009 IPT)
Tool: #4 (0.1875 2 Flute Carbide TiAlN, 0.1875 in.)
Other: Stepover: Adaptive
Allowance: 0.0000 in., Tolerance: 0.0010 in.
Time: 0:00.0
I need to change that tool anyway as surface tool selected is a square end mill. Here is some additional info on the model/file:
The first 11 operations simulate well.
The underlying 45 degree chamfer geometry and chamfer surface recognition looks good for the last 7 ops ... but I get no cutting in simulation.
It is possible that the problem might lie with my inexperience with tool management.
AFR picked surface milling for these seven chamfers, but did not pick the 45 degree chamfer tool I have defined in my crib
and I am having trouble getting the chamfer tool substituted into the operations.
When I go to the Operations List, double click the tool I want to swap for my chamfer mill ... the Chamfer Mill tool group is not there:
This is only my third project with FeatureCAM and I am likely missing something.
Any suggestions on a work around to get the chamfer tool into play here and help me get back on track?
Thank You for your time and assistance!!!
Bruce
Robert,
Again you were right on! Thank you for the good ideas. They were very helpful.
I wasn't able to get chamfers working by creating manual curves on my chamfered 3D model, but I dropped back to the previous model without chamfers and used this procedure and was able to select all the .020 edgesurfaces I needed.
That is big progress.
Now out of 37 chamfer operations, 5 fail with the identical errors.
The bosses are equally spaced at .200 using the same .1875 chamfer mill for all. The same curvature plays in other places. Not sure about that.
Also, "You are using a negative thickness that is greater than the tool's tip radius" has me scratching my head.
How a 'negative thickness' could be greater than the tool's tip radius' (.005") leaves me sure I am really missing something in the definitions.
I am almost there.
Any further suggestions as to how I might mitigate this "negative thickness" error?
I appreciate your good help!!!
Best regards,
Bruce
Robert,
Excellent suggestions! Thank you!
Going IFR, picking intersecting surfaces to chain curves to build the features got me three perfect depth chamfers and smooth simulation on the chained straight and rounded sections. NICE!
On the other five edges to go, I have tried for a couple days to get curves at the surface intersections and I am encountering two types of issues in creating the necessary curves.
The first is that I select two surfaces and instead of building a curve at the intersection, it creates multiple vertical lines on one of the faces:
Selection:
When I hit finish ... I am creating a string of vertical lines under where the curve should be from the intersection of the two faces, but trying repeatedly, I just can't seem to get the curve to form at the intersection.
I click on one of the vertical lines and get the message "Selected Curve36_6". So it looks like I am actually creating a curved surface defined by a string of vertical lines rather than one curve at the intersection of the faces. I have tried selecting surfaces in different orders, etc, but no luck at creating a curve at the top of the surface I can think of and still am missing something there.
The second issue is that I can create an intersection on two milled surfaces on one curved raised pad, but when I try to do the same on the next pad up, using the same procedure, I get the error that there is no surface-surface intersection.
Successful preview intersection:
Unsuccessful preview:
This is puzzling since the two surfaces were designed/milled exactly the same and I am using the same selection procedure ... the only difference is the second is .050 higher.
Can you offer any suggestions as what I might be doing wrong ... or some alternative to try to get the curves in place?
Thank you for your good assistance!
Best regards,
Bruce
SUCCESS!
Creating a curve from a surface edge worked perfectly for generating curves for all eight of the necessary chamfers in my test model:
With that command, I generated the curves, features and had the simulation working in ten minutes!!!
Thank you for the great suggestions and learning curve help! I really do appreciate that.
--------------------------------------------------------------------------------------
Let me ask one final question:
We made a run of this test model on an Okuma MC-V4020 VMC today. The Op suggested that we first run the post with a +4" Z elevation offset just as a check. About a third of the way through the machine suddenly started running at excessive speed. He was right on top of it to shut it down and he quickly found that a subroutine that was created at the end of the code had an F30 command rather than the F0.0187 posted at the beginning for that tool feed. In DelCAM I had set the feed for this tool at 30IPM ... which evidently was translated to F0.0187 at the front. So far my local/net searches haven't turned up any detail on this conversion factor yet ... but F30 is around a 1600X feed rate increase. It was good he was right on top of it given the impressive throw weight of this machine.
Original Feed parm:
but when the subroutine was created it evidently picked up "30" as the speed rather the converted units.
He replaced the F30 with the original feed parameter and the rest of the code ran properly.
The Op saved me breaking an expensive end mill today and I would like to return the favor by debugging the problem he has quietly been taking care of for a while now.
Can you point me in a direction that I could work towards a fix for him? (Maybe something as simple as precluding these subroutines from being generated?)
I appreciate all the great help!!!
Thank you!!!
Bruce
I ran a search in the Okuma post and I didn't find an G94, but I did find a G95 right square at the beginning.
Which I found was "per revolution" after a little checking.
So it seems that the post processor macro generator simply missed building the macro's F command with an IPR parameter or there is some other FeatureCAM parameter I don't have set properly up front when the post is produced to keep macros in IPR terms.
When I get back Monday, I will re-run the post with macros disabled and check to see if the code that gets put back at the CALL points are in IPR or IPM. The CALL only happens twice so it only costs 50 extra lines of G-code for this run.
(Will also double check that the model was started under the "Mill" selection. Maybe FeatureCAM posts G95 for lathe and G94 for mill and I ran the sim just after someone else used FC for lathe and I messed up for not checking that it was set for "mill"? That's easy nuff to scope out.)
Your comment was helpful as I am still going up the G-code learning curve and I had not caught those commands. Appreciate that!
Thanks! More later.
Bruce
