Pierce point bump.

[eibmal]

Hi group.
Does anyone have any ideas on eliminating the bump left by the pierce point. I run a hypertherm 1250 on a plasmacam. With finecut consumables on 14 gauge and smaller this bump is hardly noticible. On thicker material 1/4" and 1/2" using 80amp consumables the bump is more evident.
Thanks.

[jimcolt]

You need to enter a "lead in" length......the pierce point should always be in scrap material, not on the part itself. If the lead in length is zero...you will get a divot!

Jim Colt

[eibmal]

Hi Jim.
Thanks for the fast reply.
I do have the default 0.15 lead-in set if the Pcam software. I can see the lead in being cut. I also have the gap at end of loop set at 0.01 I have tried cutting with no gap, but still get a small divot. Air pressure is set at 70psi , a 3stage dessicant dryer with an add on PCP Group dryer insures clean dry air. Are there any options I can try to solve this problem.
Thanks.

[jimcolt]

Can you post a picture of the bump your are describing......try a longer lead in.....perhaps .2 instead of .15....see if that makes a difference.

Jim

[eibmal]

Hi Jim.
This is a 2" cicle with a 1" cut out. 0.25" New mild steel. Cut with 80amp alsmost new consumables at 60imp. I increased the lead-in to 0.2 but still get the divot. Cutting at this speed produced very little dross and a not bad taper.

Thanks.

[jimcolt]

Ahhh.....that is not the pierce point. It is either the 90 degree corner where the lead in has to turn a sharp left to start the circle......or, it could be the shut off point at the end of the cut, right at 360 degrees around the circle.

1. Increase the machines corner acceleration rate.....a bit at a time. This will minimize the divot if it is caused at the lead in intersection. If the acceleration rate is too slow...the machine dwells slightly at this point.....and the plasma burns a waider kerf.

2. If it is caused by the end of the cut....there is a setting in plasma cam that keeps the arc on after the motion stops at the end of the cut.....it is called "continue cutting after stop".....but it is designed for use with thicker materials to allow the part to drop (to let the lagging bottom of the plasma arc catch up and cut all the way through).....set this setting to zero....and that also should help.

Also.....You will like these parts on 1/4" a lot better if you match the power to the material thickness. I would use 40 Amp shielded parts for best quality on 1/4"...the speed will be slower, but the cut edge will be square and more accurate. 80 Amps should be used above 1/2" for its best quality.

Jim

[eibmal]

Hi Jim
I have tried changing the corner accel 0.1 at a time up to the max of 1.0. Each cut 0.1 more than the previous one. I also set contin cut after stop to 0. Best setting was with the corner accel at 0.5 However the improvement is not significant. I do not have 40amp consumables, but will get some on Monday. Any other suggestions?
Thanks.

[jimcolt]

I think the 40 Amp process will help. Think about what it is doing.....it goes through the lead in, then decellerates to 0 ipm, turns left, then has to accelerate along the radius of the circle. With a less aggresive process (40 Amps vs 80 Amps) it should produce less of a divot. Let us know how that works.

Jim

[eibmal]

Thanks.
I'll let you know the results.

[eibmal]

Hi Jim.
I have now tried cutting the 0.25 plate with 40a . There is an improvement in the problem. I would say it's about 50% better and the quality of the cut is also better. I called plasmacam and asked if there is a way to eliminate this problem. They have said that it will never be 100% gone.
Thanks.

[jimcolt]

You can eliminate it with a precision cnc machine and a high definition class plasma....however you would have over $100 k invested in the equipment. You are doing very well with an entry level plasma and cnc machine!

Jim Colt

[ALLOHIO]

Try moving your lead in behind the cut so it flows better that has worked for myself.

Paul

[eibmal]

Thanks for the reply. Could you elaborate on exactly how to do this.
Thanks.

[weldguy]

Thanks for the reply. Could you elaborate on exactly how to do this.
Thanks.

Check this post for a diagram showing a smoother lead in.

http://plasmaspider.com/viewtopic.php?f=45&t=877

The sharper the corner, the more deceleration most software will introduce causing the torch to slow down and create imperfections in your cut. Keep your lead ins flowing straight as possible for best results.

[planetxfred]

How about having the leadin come in tangent to the circle? that should reduce or eliminate the speed change on the corner. I have done this by stretching the start point to provide a smooth lead in. I don't know if there is a seting in the PCAM software to do this automatically.
Fred

[vmax549]

Just curious but are you running a leadout as well ? It may help to move the problem away from the cut area IF it is a stop problem so it does not affect the part.

Also IF you runn servos on your machine they may be overunning the stop point of the leadin and correcting back. May need to check tunning if you are useing servos.

Just a thought, (;-) TP

[AnotherDano]

Has anyone found a way to manipulate the pierce point in PlasmaCam that works?
I'm having a heckofa time with problems like this. Small cutouts and highly detailed areas especially!

[eibmal]

Thanks for all the help from members of the group.

For anotherdano or any other PCam user.... Changing the lead in has almost eliminated any ridge or divot from the cut path. After reading a post on lead in, I was able to get a way better cut. Here's how I did it. When cutting art work the kerf may not be that important. In path conversion set the kerf to 0. With your drawing in Pcam , convert the drawing to a cut path. On any cut, it is better to have the torch follow the lead in, in the direction of the cut. Try to eliminate any 90 deg lead ins. Zoom in on the lead in created by the software. Then from the edit drop down menu, select edit path. Your cursor will now be on the lead in. You can move your cursor to change the angle or length of the lead in. .
Hope this helps.

Thanks.